Altium questions

[Faringdon]

Hi,
Please may i open this for all Altium problems? (save creating new post each time).

I am not able to put a component from a certain library in to  my schem......i cant detect this library even though its there. It is in fact the original lib from which the schem was first created.
Strangely , i made my own schlib and it can see that.
How do i make it see this other sch lib?

[jc101]

Have you tried the manual?

https://www.altium.com/documentation/altium-designer/schematic-searching-placing-components

Is the location of the schematic library within the project search path?

https://www.altium.com/documentation/altium-designer/accessing-defining-managing-project-options#search_paths

[Faringdon]

Thanks, that was really helpful.

Locating centrum of a dpak footprint....
Ive now just copied a DPAK footprint into my own library...but its centrum is not marked, so i cant drop it on the centrum in the footprint editor.
Do you know the best way to find the centrum for a DPAK?....in Eagle i just draw construction lines and where they cross is the centrum...is that the right way to do it in Altium?.....as you know, the centrum must be known, and marked,  as its needed for the pick n place coordinates.

[Faringdon]

Hi,
Noddy version of Altium
Are there any youtube vids or docs, which give "altium for contractors"...ie people who just need to get a small board done and dont have the time to get into the myriadical depths of Altium?
Altium could do with a cut down  "noddy" version...so contractors can just do something quickly, in the initial period when they dont have time to delve into the depths of PCB layout jargiography.
Or is there a "noddy altium" video , which shows you just how to do the basics, manually, in Altium?
Like an EAGLE  version of Altium......Eagle is learnable within a day.

[Faringdon]

Copy and paste in footprint editor
Hi, I am doing right click copy paste, and CTRL C, CTRL V, but they dont always work.......i am trying to copy a line and move it 2.8mm to the left......the copy and paste only seems to work if you paste right over the top of the line that you just copied, is this correct?

[jc101]

When you do ctrl-v the next click is on the object you want to copy, and picks the pickup point. Then you can go to where you want that reference point to be and paste it. So you select the part, copy, click the reference point then paste it. For a line pick the end of the middle, then move as needed and click to place.

It’s intuitive after a few. You can do the same with multiple parts too.

[ajb]

Locating centrum of a dpak footprint....
Ive now just copied a DPAK footprint into my own library...but its centrum is not marked, so i cant drop it on the centrum in the footprint editor.
Do you know the best way to find the centrum for a DPAK?....in Eagle i just draw construction lines and where they cross is the centrum...is that the right way to do it in Altium?

In the footprint editor, Edit > Set Reference > Center will set the component reference to the geometric center of the pads.  This isn't always what you want (for example if all of the pads are to one side of the component), so you can also do Edit > Set Reference > Location and then click where you want the reference to be.  It's not necessary to move the primitives around in the footprint to center them, although you can do that.  Drawing construction lines to establish geometry is perfectly valid in Altium, although

as its needed for the pick n place coordinates.

Altium will generate a pick-and-place file without a marked center, just based on the component reference, but a marked center is definitely good practice. 

Noddy version of Altium
Are there any youtube vids or docs, which give "altium for contractors"...ie people who just need to get a small board done and dont have the time to get into the myriadical depths of Altium?
Altium could do with a cut down  "noddy" version...so contractors can just do something quickly, in the initial period when they dont have time to delve into the depths of PCB layout jargiography.
Or is there a "noddy altium" video , which shows you just how to do the basics, manually, in Altium?

Ehhh, I don't think the Altium team need anything else to distract them from the core product  .  In all seriousness, Altium is a much more sophisticated tool than Eagle.  There's vastly more capability and baked-in automation of data handling, and while it's easy to say 'but I never use X or Y or Z', the application workflow still depends on those things being in place, and adding an option to remove them makes the software more complex, not less.  Even if it's simpler for the user, it's more complex to develop, meaning more opportunities for problems to crop up.  (It's something of a law of software development that the simpler it is to use, in terms of effort:results, the more complex it is to write and maintain.)  Aside from which, you'd have to decide which of those features a "contractor" potentially needs, which first requires deciding what kind of design work a "contractor" does.  The answer to the latter is "could be anything" and therefore the answer to the former is "all of them".

If you continue with Altium and put some effort into understanding the workflow I think you'll find that it's largely worthwhile in terms of productivity and capability in the end.

[Faringdon]

Multiboard project and checking PCBs and SCHEMS are all synch'd?
Hi, Am modifiying a 17W SMPS on a PCB, which is one of three PCBs which all belong to the same multiboard project. The circuitry on the three PCBs is across some seven different schematics.
I have done some changes.....how do i push them through to PCB?...is it hit Design then Update..?....

When i have done this, and hit "execute changes", then close......then when i hit  Design -> Update again....   ....shouldnt it tell me that the schematic i am working on is correspondent with whats on the PCBs?

How do i know if the seven schematics have components, designators,  and nets on them, which correspond to what's on the three PCBs?

[Faringdon]

Unrouting nets in PCB editor
Hi, Currently re-laying out the circuitry on a PCB…need to delete all polygons and nets and stitching and thermal vias on this PCB. How do I do this? How do I know if a thermal via has been done as a component, or just added in to the PCB?…if it’s a component, then as you know, I cant just delete it.
Some of the traces, when i highlight them and click properties, they say "N/A" to the net name...does this mean they are not nets, and that i can just delete them......i ask because in Eagle, you cannot delete nets, because the PCB and SCHEM then become desynchronized. Is it same in Altium?
Now, when i delete the polygon, it leaves its outline there, and even offers me to repour...but i just clicked the "bin" to delete it? How can i get rid of polygon pour and its outline?

[Faringdon]

Moving net wires about in SCM editor
Ive searched but cant find a good video on moving nets about in Altium schm window. (eg when tidying up a schem) Its nowhere near as easy to do as Eagle. In Eagle, it “knows” what you want to do, and you just grab net wires, and move them about as you please…Altium is far less easy with this…it doesn’t seem to know where you want to move things, and moves things in to “silly” places. Takes much longer. What am I missing?

[Faringdon]

Stop line snapping in Library footprint editor
Hi, I just tried to draw a 0.2mm silkscreen line outside of a courtyard “box” line on mech 15…..it wouldn’t let me do it….it constantly kept snapping to the mech 15 line….how do you make it snap to the grid lines at 0.1mm, instead of to the mech15 line?

[thm_w]

Unrouting nets in PCB editor
Hi, Currently re-laying out the circuitry on a PCB…need to delete all polygons and nets and stitching and thermal vias on this PCB. How do I do this? How do I know if a thermal via has been done as a component, or just added in to the PCB?…if it’s a component, then as you know, I cant just delete it.
Some of the traces, when i highlight them and click properties, they say "N/A" to the net name...does this mean they are not nets, and that i can just delete them......i ask because in Eagle, you cannot delete nets, because the PCB and SCHEM then become desynchronized. Is it same in Altium?
Now, when i delete the polygon, it leaves its outline there, and even offers me to repour...but i just clicked the "bin" to delete it? How can i get rid of polygon pour and its outline?

If you need to delete everything, you can use the filter tool to filter out polygons, then just highlight everything and press Delete. Same with the vias.
https://www.altium.com/documentation/altium-designer/pcb-filter-panel?version=18.1

If a trace has no net, maybe the net has been deleted from the schematic at some point. If you delete the trace in the PCB you are not deleting a net. Again you could use filter and find no-net traces, select them all and delete if you want.

Polygon just press delete to delete it. You can also go to the Polygon manager and look there.
https://www.altium.com/documentation/altium-designer/pcb-dlg-polygonmanagerformpolygon-pour-manager-ad?version=22

[thm_w]

Stop line snapping in Library footprint editor
Hi, I just tried to draw a 0.2mm silkscreen line outside of a courtyard “box” line on mech 15…..it wouldn’t let me do it….it constantly kept snapping to the mech 15 line….how do you make it snap to the grid lines at 0.1mm, instead of to the mech15 line?

https://www.altium.com/documentation/altium-designer/pcb-grids-system#!the-snap-points
https://www.altium.com/documentation/altium-designer/sch-dlg-form-getcoordchoose-a-snap-grid-size-ad?version=21

[Faringdon]

Components in schem are from which library(s)?
Hi, Thanks,  Just trying to find out how to get a list of the components on a schem page, and what library they are from?

[thm_w]

Components in schem are from which library(s)?
Hi, Thanks,  Just trying to find out how to get a list of the components on a schem page, and what library they are from?

If they are defined, and not any, I think its in the component parameter table?
https://www.altium.com/documentation/altium-designer/workspacemanager-dlg-parametereditorformparameter-table-editor-ad?version=22

[temperance]

RTFM

Or do this



or

https://www.altium.com/documentation/altium-designer/tutorial-complete-design-walkthrough

or

https://www.ece.ufl.edu/academics/altium-designer-video-tutorials/

It's all there and the online help made by altium is actually very usable. But as usual, you will not bother to try and find answers by yourself and revert to a forum instead with a zillion questions which you can answer by yourself if you would put a small tiny bit of effort in studying the manual. Don't be scared now. You might learn something. 

[Faringdon]

Unknown pin error...cant push schem to PCB
<<EDIT...NOW SOLVED.....Altium was somehow putting in A footprint from another library....which had the same name and shape etc......it was in a  different library, so i dont see how Altium got confused...i think this is a bug in Altium?..END OF EDIT>>
Thanks, ive done a number of tutorials and will do more.
Just downloaded a 7447714470 inductor model for Altium (from the wuerth website), with 3D, and put it into my library...then put it into the schem, and pushed it through to PCB...but it gives an error "unknown pin L101-1".....i dont understand this.....the pin is  clearly in the SCHLIB, and its clearly in the PCBLIB....so howcome it says its "unknown"?
....Ok, now solved by deleting the inductor from schem..then pushing thru' to PCB...then re-inserting the inductor in schem...then pushing thru' to PCB all over again....seems like a "round the houses" way of doing it?
....Now getting  "unknown pin" error with another inductor...and this time it wont solve like the above...anyone know how to solve?
...Now solved that, but strangely the silkscreen dot  which marks pin one of the inductor, isnt appearing in the layout editor....do you know why?
(its a "dotted" inductor).

[jc101]

Any duplicated part identifiers?  DId you run an annotation on the schematic too?

[Faringdon]

Project has "closed up"
Hi, When i previously opened the multi board project, it showed me all the files in it in the Project window.....now i cant see those files, and can pretty much only see the project name....how do i get the "opened up " project view back? I cant open the files in the project at the moment...the SCM and BRD files.
<<EDIT NOW SOLVED by closing out of altium and re-opening again....END OF EDIT>...is this the best way to do it?

[Faringdon]

Component designators too big in PCB window
<EDIT ok now solved with link below END OF EDIT>>
Hi, I tryed to reduce them in the footprint library, but it doesnt work.......did the "find similar objects" thing.....set string type to same, and text to same, but still not getting the designators reduced in size...do you know how......they are 1.524mm high.....we want them 0.5mm high text.
<EDIT...THE following doesnt seem to work...the EDIT command in PCB LIST is not there.
https://www.google.co.uk/search?q=reduce+size+of+component+designaotr&sxsrf=APwXEddbF4ViiWKddIraqoI_Ibi6GiLc-w%3A1683834569685&source=hp&ei=yUZdZM_VJuqYhbIPo-qWuAk&iflsig=AOEireoAAAAAZF1U2abCzJm0zitwQ9oUAwaHpTqHB7r1&ved=0ahUKEwiP3ojLhO7-AhVqTEEAHSO1BZcQ4dUDCAs&uact=5&oq=reduce+size+of+component+designaotr&gs_lcp=Cgdnd3Mtd2l6EAMyBwghEKABEAoyBwghEKABEAo6BAgjECc6BwgjEIoFECc6CAgAEIoFEJECOhEILhCABBCxAxCDARDHARDRAzoLCAAQgAQQsQMQgwE6CwguEIoFELEDEIMBOg4ILhCABBCxAxCDARDUAjoHCAAQigUQQzoTCC4QigUQsQMQgwEQxwEQ0QMQQzoFCAAQgAQ6DQgAEIoFELEDEIMBEEM6CggAEIoFELEDEEM6CggAEIAEEBQQhwI6BggAEBYQHjoICAAQigUQhgM6CAgAEBYQHhAPOgUIIRCgAToICCEQFhAeEB06CgghEBYQHhAPEB06BAghEBVQAFiqJ2CBKGgAcAB4AIAB3wGIAakqkgEGMC4yOS41mAEAoAEB&sclient=gws-wiz#fpstate=ive&vld=cid:cbe6c11d,vid:tF64-xMrqLw

END OF EDIT>>

[thm_w]

Project has "closed up"
Hi, When i previously opened the multi board project, it showed me all the files in it in the Project window.....now i cant see those files, and can pretty much only see the project name....how do i get the "opened up " project view back? I cant open the files in the project at the moment...the SCM and BRD files.
<<EDIT NOW SOLVED by closing out of altium and re-opening again....END OF EDIT>...is this the best way to do it?

Surely you'd just double click the project folder... no 

https://www.altium.com/documentation/altium-designer/projects-panel?version=19.0

[ahbushnell]

Why a special topic for Altium questions?  Plus it means we can see if it's a question of interest if there is not a unique subject line.

Andy

[Faringdon]

Cant select resistor or its designator in pcb editor
Hi, Altium keeps selecting the chip on the bottom layer whenever i try to select the res on the top, or its designator......Eagle has a "next" button for this....does Altium?

[Faringdon]

Hi, PCB routing
Just routing up a PCB now…plenty of google/manual  searches not revealing the following…
How to pick the via size when you change layer
How to actually properly change layer
How to set the clearances for the various net class’s

[Faringdon]

Keep getting kicked out of licenced operation
Hi, got kicked out of the licence in Altium again....how do i get back to the licence page?....i am just doing it by going on a 10-15 minute wild click splurge until i end up back at the licence page...but how to get there quickly?

[temperance]

AD prefers to select the component on the current active layer. (active layer is the active layer tab. See bottom of the PCB screen)

In general, this applies to anything you want to select. Traces, planes,... You first have select the layer.

[Faringdon]

Lost contact with PCBLIB
Hi, Yesterday, i sucessfully linked in the PCBLIB, and was happily putting footprints into my schem sybols....today, i cant find the PCBLIB library....i know which folder its in...but i cant make Altium see it...do you know how to do this?
eg this vid is useless, as Altium cant see the library..

...Now seem to have done it....i opened the PCBLIB by "Add existing to project"...then somehow, a dialog box opened, and i searched for that PCBLIB, and somehow linked it in......i dont think i  know where that dialog box came from, so i hope i remember for next time...........the "search paths" TAB thing, which was working great yesterday, suddenly was useless today.

[thm_w]

Why a special topic for Altium questions?  Plus it means we can see if it's a question of interest if there is not a unique subject line.

We don't need hundreds of threads for this, I explained before. Its just a general tips and questions thread.

Cant select resistor or its designator in pcb editor
Hi, Altium keeps selecting the chip on the bottom layer whenever i try to select the res on the top, or its designator......Eagle has a "next" button for this....does Altium?

No but you can switch to single layer mode (shift+s) and then choose either the top or bottom layer, that might help.

Hi, PCB routing
Just routing up a PCB now…plenty of google/manual  searches not revealing the following…
How to pick the via size when you change layer
How to actually properly change layer
How to set the clearances for the various net class’s

Press tab when placing a via/trace then you can edit the default values, like width or hole size, etc. Then this should be saved as default for your next placement.
Change layers: https://resources.altium.com/p/my-favorite-altium-designer-keyboard-shortcuts-and-viewing-features 
Clearance: https://designhelp.fedevel.com/forum/main-forum/altium/2093-how-to-set-clreance-design-rule-between-two-net-classes

[temperance]

That video about those footprints you provided is utter rubbish. Did you read the manual? Did you follow the video courses I provided. No you didn't...

So here is an other one:


Try this, it works...

Altium itself provides a step by step video guide on YT. It get's you from discovering how things work to creating manufacturing data in no time. Just a couple of hours.

[Faringdon]

Polygon pour with no thermal reliefs
Hi, I wish a certain polygon pour to have no thermal relief to a component pad and a via. Do you know how?

[jc101]

->

Done in the design rules.

[Faringdon]

EDIT..pse see below..
Hi, Do you knwo how to download footprints to Altium from Ultra Librarian
I have done the following
https://youtu.be/r1tv_wz_uY0?list=PLkqC31nn-k7mujTz7vwejPDVVnKrZG4A4
..many times, but it just crashes Altium every time....and you cant even close Altium ...it says its "stuck on a breakpoint"
You have to close Altium via Task Manager and re-open Altium.
Using Altium 22.10.1
EDIT.....Ultra librarian now works....it looks like it logged me out of the licence, but still carried on working , but in a "strange mode"...END OF EDIT

It always seems to say i am using a licence...but how do you really know you are?

[jc101]

Have you tried to run it as a script?

https://app.ultralibrarian.com/content/help/?altium_designer.htm

Not used Ultra Librarian, but for PCB Libraries, this is how things get generated into their own library.  I can then copy and paste them into my own libraries.

Edit to add that the PCB Libraries generation does all the 3D models automatically, which is quite handy.  Not free, though.

[PlainName]

Do you knwo how to download footprints to Altium from Ultra Librarian

I found it simpler and more consistent to not bother, and just create my own. The datasheet for the component will have the info you need, and you will use your in-house standardised layers (as opposed to someone elses preference which is different to yours). As an additional check, applying a 3D model shows whether the pads line up (not foolproof, but two or more people making the same mistake isn't that common).

[Faringdon]

Gerber and drill files:
Thanks, Do you know which files in  the attached are the drill files to send off with the gerbers...the Altium "camtastic " files seem to be gerbers?

[PlainName]

Send off the one named 'BOTTOM PCB'.

[thm_w]

Gerber and drill files:
Thanks, Do you know which files in  the attached are the drill files to send off with the gerbers...the Altium "camtastic " files seem to be gerbers?

You need to generate the NC drill file, if you want to do it manually: https://www.altium.com/documentation/altium-designer/workspacemanager-dlg-drillsetup-formnc-drill-setup-ad?version=17.1
You can see the list of files it would generate.

edit: might help if you turn on file name extension in windows so you can see the .extension

[Faringdon]

Thanks, when you do it in Eagle, there is only one drill file to send for manufac...why not with Altium too?

[jc101]

You have configured an OutJob?  There you can generate all the files needed for manufacture, my drill files come out as .txt

https://www.altium.com/documentation/altium-designer/streamlining-generation-of-manufacturing-data-with-output-jobs

[Faringdon]

Thanks..
Schematic shuffling
When i try to compress/tidy my schematic, it doesnt let me do it well..in Eagle it just allows you to select and stretch and move the wires and components...and when theyve been moved, it knows exactly how to leave them connected...but Altium leaves you with a tangle to untangle......how do you best do it?
Highlight net in schem
In Eagle, you can select any net in the schem, and go right click, and click "show", and it highlights that whole net, wheresoever it may go..... how do you do this in Altium?

[thm_w]

Drag: https://www.altium.com/documentation/altium-designer/sch-cmd-dragdrag-ad?version=18.1
Look at the tips at the bottom.
If you can, try to group things into functional blocks. Then you can drag those blocks around and not have to constantly re-wire.
I use a huge sheet as I don't care about printing out the schematic, but won't work for everyone.

Highlight: alt click https://www.eevblog.com/forum/altium/highlight-the-same-net-in-a-schematic-altium-17/

[Faringdon]

View configuration panel:
Hi, How do i get the "view configuration" panel back as a panel, rather than stuck to the bottom of the window as attached?

[Faringdon]

Import to Eagle
Hi, Does anyone know how i can import a PCB and schem into eagle, so i can design rule check it and gerber it up?....in Altium, i have lost the "view configuration panel"....and i cant check the layers properly.
The  layers are stuck to the bottom of the display, and not in their usual popup panel.

[jc101]

Did you not setup the design rules in Altium? Correctly set should be exceedingly hard to generate a design that breaks the rules. It’s all done in real time as you lay out the PCB.

The panels you can drag from memory from their header bar. The layers have always been on the bottom for me. Shift-S goes into single layer mode and again to go back to all layers.

[Faringdon]

Thanks, its the "view configuration" popup.....its just gone...i click "Panels", then "view configuration"...and nothing shows up...every other time it was there...now gone...do you know why?

I actually think what I have here is a  bug in Altium….because the “view configurations” popup has simply vanished…….whereas I have been getting it for the last few weeks….without problems.
I have had multiple other issues with other features in Altium…eg the “direct pour” feature has been undoing itself sporadically…..i think when you are a beginner in Altium, you have irregular click sequences within it, and that this sparks off bugs…like what I am seeing now……the “view configurations” panel actually opened first thing this morning…but when I (admittedly roughly) tried  multiple times, to dock it to the side bar…it then  just disappeared…and I haven’t been able to get it back since. This surely is a bug, IMHO.

[jc101]

System-> Preferences-> System > View, hit reset under Desktop on the right.  Should reset the positions of the panels etc.

[Faringdon]

Hi, The Layer views at 15:50 if this  video


...can you get them with an assigned shortcut key?...eg  " ALT, L", whatever?
Otherwise constantly having to go off and left click on the thingy, then left click on the selection thingy, is going to get a bit long winded

[jc101]

Help -> shortcut keys, have a look in there. 

I hardly go into that menu post initial PCB setup, Shift-S goes into single-layer mode, and the + - on the numeric keypad skips between the layers.

Or here for the list of PCB editing shortcuts... https://www.altium.com/documentation/altium-designer/shortcut-keys-pcb-editors
For the layer menu, press L

You can also right-click a layer and choose to show or hide it.

[Faringdon]

Hi, Please could anyone help with the following..or know of video links for it?

1…How can you be sure your design rule setting don’t get wiped?....can you save it as a file?
2…Just pushed my components to PCB, and many f them are coated in green crosses, and appear totally green when I “scroll out”. Do you know what this is?
3….I added a  Mech Layer 22,  which I used as a component courtyard in the PCB  component editor, but now mech layer 22 has mysteriously disappeared from the “view configurations” panel…do you know why or how?
4…In schem editor, I routed a track over another one, and it joined to it, but that wasn’t wanted…how avoid this.?
5…In PCB component editor, I am trying to move a SMD pad by just 0.1mm…but it wont let me, even though the grid is set for 0.1mm…..it instead snaps the pad to the nearest line….how to avoid this?
6…How do you add a designator to the component footprint?
7…If you want to place a keepout in the gap between the pads of an 0805, is it just a case of drawing a rectangle in the gap, made of “keepout” net?
8…I wish to make a SOIC 8 footprint by setting the grid to  1.27mm, then just move the pads by one “jot”, to get the line of 4 pads…..but it wont do it..it woves the copied pad to the nerest gris mark, rather than just moving 1.27mm in the Y direction. How to solve?

[thm_w]

1 - Design rules are part of the PCB file, and you should be doing proper version control or at least a regular backup of that file.
2 - Do design rule check and it should tell you in the messages, maybe height is too high, outside of the room, etc. its some violation. Tools -> reset error marker also might help temporarily
4 - Undo and reroute somewhere else
5 - Change snap settings or move the component via the X-Y numbers in the component properties box  https://my.altium.com/altium-designer/getting-started/snap-options-pcb
6 - Look at an existing component that has one, its in the designator field, U? or whatever
7 - You can do polygon cutout if its specific to a pour, or change the design rules, keepout might work as well https://www.altium.com/documentation/altium-designer/pcb-region-keepout?version=21
8 - see above

[PlainName]

1…How can you be sure your design rule setting don’t get wiped?....can you save it as a file?

You can export them, and import whatever set you've previously exported. Right click the rule tree, select Export Rules (see screeny) and then select which rules you want to export.

[Faringdon]

Selecting components in PCB layout editor
Hi, Do you know how to select a component in the PCB editor, and avoid it homing in to a super-zoomed-in view of that component?

[Faringdon]

PCB Editor manipulation:
Can Altium PCB layout editor have the same  superb features as Eagle Pro?..
.When laying out in Eagle, and I want to get a component onto the mouse, so I can place it, I just type “R28” say in the dialog box, hit return, and then  R28 is stuck to my mouse, ready for me to move it where I want….Altium doesn’t appear to have this.
Also, when I want to go from schem to PCB screens, I just hit the relevant hot-keys….you can set the hot-keys as you wish. In Altium, I have to  click on the exact place so as to change between them. Also, in Eagle, you can also use a hotkey of your choice to make any particular layer_set show on the screen….very useful…none of this is poss in Altium, and so Altium is more unwieldy.
Or can these things be done in Altium?

[jc101]

PCB Editor manipulation:
Can Altium PCB layout editor have the same  superb features as Eagle Pro?..
.When laying out in Eagle, and I want to get a component onto the mouse, so I can place it, I just type “R28” say in the dialog box, hit return, and then  R28 is stuck to my mouse, ready for me to move it where I want….Altium doesn’t appear to have this.

Open the PCB panel, select components at the top, Pick All Components or those from a specific schematic you want.  Double click the part and it will be selected.  Adjust the Zoom Level at the top if the PCB panel to determine how far it should zoom in when selecting the part.

Also, when I want to go from schem to PCB screens, I just hit the relevant hot-keys….you can set the hot-keys as you wish. In Altium, I have to  click on the exact place so as to change between them. Also, in Eagle, you can also use a hotkey of your choice to make any particular layer_set show on the screen….very useful…none of this is poss in Altium, and so Altium is more unwieldy.
Or can these things be done in Altium?

Press W to pop up a list of open windows, then just pick the one you want.

Swapping layers when routing is + and - key on the keypad

Press L to get the layer viewer to pop up, you can then turn of/off groups of layers as you choose.

All of this is in the help, lookup shortcut keys.

[T3sl4co1l]

Document tabs can be cycled with CTRL+TAB. Or drag a document off to open a new window (best for multi monitor).

I always navigate components by J, C (Jump to Component), or cross-selecting them (usually to see regional grouping) i.e. select on SCH and they select on PCB.

For different queries, I use PCB Filter and List.

Tim

[Faringdon]

Getting rid of error markings---now solved
EDIT...OK...done it, it was "component clearance rule"
Hi, i have two connectors close together, i suspect there is a violation of the silk to silk setting, so the connectors are totally covered in green crosses, and i cant see the tracks and components underneath them...do you know how to get rid of error markings? (i am not allowed to move these connectors.)

[jc101]

Tools -> Reset error markers, which should clear the violations.

[Faringdon]

Layer sets manager
Hi,
I just watched a video on how to do this, but it wasnt possible.
Do you know how to define a layer set, so you can view only that set of layers?

Selection options dialog
Hi, Do you know where in Tools Prefs i can get this?....when you hover over something in PCB, and it wont select it cuzz it selects only whats covering it instead...

Move a component in PCB and track comes loose
Hi, Can you make a track auto-reconnect when you move a component and the track that was connected to it "comes loose"

Do i have to go and find something to click on always?
No hotkeys to select stuff?...takes longer to hunt for something to click on a menu....to find a component i have to click "components"...then scroll down...then find the component...then click it......takes ages!

[PlainName]

when you hover over something in PCB, and it wont select it cuzz it selects only whats covering it instead...

Just keep selecting and it will cycle through the stack of objects under the pointer.

[PlainName]

No hotkeys to select stuff?...takes longer to hunt for something to click on a menu....to find a component i have to click "components"...then scroll down...then find the component...then click it.....

From the edit menu select 'Jump' and then ctrl-click 'Component...'. You'll be shown the dialog pasted here, where you can add whatever hotkeys you want to pup up that 'jump to component' whenever you want.

The ctrl-click causes the menu item configuration dialog to open for any menu item - this is how you set up or change hotkeys.

[Faringdon]

Thanks.
Replacing all  thru hole pads with  2.5mm diameter  round pads?
Hi, I have got a 20 Watt offline flyback that ivve just layed out in Altium...but now they say thay cant wait 5 days for a PCB to come back from JLCPCB etc...so want me to mill out a  copper clad board...they say they have a milling maching which can take the  bottom copper gerber as the "guide".

...So to do the PTH components, and the vias,  i need to replace their pads with 2.5mm round pads so i can drill them with a 1mm drill.

How, in Altium, do i replace all thru holes with a 2.5mm round pad on the bottom layer?......is it just a case of "place", "circle", "bottom copper"........and do that for every PTH?

[jc101]

Speak with some UK PCB makers who could probably turn it around in 24 hours.
Cambridge Circuit Company could help. Won’t be that cheap…
https://www.cambridge-circuit.co.uk/

Stand a better chance of getting a decent board than cobbling something together.

[T3sl4co1l]

https://www.altium.com/documentation/altium-designer/working-with-the-query-language

[tooki]

Thanks.
Replacing all  thru hole pads with  2.5mm diameter  round pads?
Hi, I have got a 20 Watt offline flyback that ivve just layed out in Altium...but now they say thay cant wait 5 days for a PCB to come back from JLCPCB etc...so want me to mill out a  copper clad board...they say they have a milling maching which can take the  bottom copper gerber as the "guide".

...So to do the PTH components, and the vias,  i need to replace their pads with 2.5mm round pads so i can drill them with a 1mm drill.

How, in Altium, do i replace all thru holes with a 2.5mm round pad on the bottom layer?......is it just a case of "place", "circle", "bottom copper"........and do that for every PTH?

You modify the footprints. Then you update the PCB with the updated pads.

No, you don't place fucking circles. You edit the pads.

Alternatively, if it's a one-off change (i.e. you want to manually override without modifying the footprints (meaning that if you do update the PCB from footprints, your overrides will be lost), you can just select all the pads and change them manually.

But I think this whole idea of milling a board is a profoundly bad idea.

[Faringdon]

NET CLASSES
Hi, I have just defined  some net classes in the PCB editor....but then when i pushed through some changes from scm to pcb, the net classes disappeared.
How do you define net classes which dont disappear?
....OK, end of this vid seems to address this...

ill just check

[tooki]

Either deselect those from the ECO when updating the PCB (every time…), or do it the “right” way by attaching them as parameter sets in the schematic editor. Those are these lollipop-shaped objects you place on a wire. You can (among other things) apply net classes (so that you can write net class specific DRC rules)l or you can even apply rules directly to the parameter set. It’s also closely related to how you define differential pairs. I’ve used them, for example, to define which connections are 50 ohm controlled-impedance traces.

https://www.altium.com/documentation/altium-designer/specifying-design-requirements-during-design-capture

[Faringdon]

Thanks, must admit i dont like the lollipops  (parameter set things).....soetimes i want a certain net to be a member of two different net classes, and having those lollipops all over the place really confuses things IMHO.
I am currently defining net classes in the schem by having a separate schem just for "blankets", i then put a net and a net label in there for every net i want in that net class....then put the "lollipop" on that...then push through to pcb...but this takes ages.....

[tooki]

I know what you mean, it can get cluttered. If anyone knows a better way to apply a parameter set to a bunch of wires simultaneously, please speak up!

[T3sl4co1l]

I do it like this sometimes.

Tim

[asmi]

Speaking of which - does anyone know if it's possible to have stuff created by xSignal Wizard (like DDR3 classes, xSignal groups, etc.) to be somehow transferred to schematics such that ECO would stop complaining about them and offering to remove them? I know about disabling such removals in project options, but I would like to avoid using such broad-reaching tools whenever possible.

[Faringdon]

Updating from library & Clearance design rule
Hi,
This isnt working....im doing it but it doesnt happen.
I have these SMD chip resistor footprints with a keepout rectangle in between the pads, so that copper pours never go between the pads.....but Altium thinks the keepout is a track....and is moaning that its too near to the pad....(<0.3mm which i set as min clearance). So anyway, i modified all the keepout rectangle so they are more than 0.3mm away from the SMD pads...and clicked to "update from librariaies"...but it hasnt happened......and still the design rules check is painting the entire pcb layout editor green with error markings which obviously shouldnt be there.
Anybody know how to solve.
This must be an altium bug?....a "keepout" is a  keepout...it is not a track...why does altium think its a track?
Altium also seems to think that my "mech 22" layer (my component courtyard layer) is a track and is flagging clearance issues with it.....obviously some random mech layer is not a track....and shouldnt be exciting the clearance rules....this must be a bug?
It really breaks your momentum when you have to keep stopping a layout to try and search for whats going wrong. You have to workout what jargon Altium is using for the feature, then try and get behind it. I keep breaking off for google and altium rule guide sessions, but it often doesnt do much good.

Altium videos like this should be clearing these issues up...but are , to be honest, not very good...


Ive done some googling, but cant find, for the love of the almighty, why altium is doing clearance rules between mech 22 and some pad copper...and turning my pcb layout editor green with error messages, which obviously should not be there.

A clearance rule..surely, should only mean clearance between copper nets?....is this an altium bug?

[PlainName]

I have these SMD chip resistor footprints with a keepout rectangle in between the pads, so that copper pours never go between the pads.....but Altium thinks the keepout is a track....and is moaning that its too near to the pad....(<0.3mm which i set as min clearance)

The keepout is working fine - it is keeping out the pads, which are part of the signal layer and thus shouldn't intrude on keepout areas.

[Faringdon]

Thanks, but i put the keepouts there...and they dont intrude on the pads.

[PlainName]

If you right click the keepout object, you can change the restrictions so it ignores pads.

I think keepout also uses the global clearance, so if you want it right up against something then you might have to make a specific keepout clearance rule:

https://www.altium.com/documentation/altium-designer/object-specific-keepouts-pcb#!keepout-clearance-rule

[Faringdon]

Reconnect tracks
Hi,
When you move a component and its track comes disconnected, how do you make that track auto-reconnect?
Disable everything in Altium
Hi, Am trying to route up a simple PCB...and Altium is making the track dance all over the place as i route it...it wont let me put the track where i want it.......how can i disable absolutely all these extra features in Altium?, so that i can then put them back , individually, as and when  they are required.....for this simple board, i just need Altium to act like Eagle does anyway.
Altium videos
Have now watched shedloads of altium videos, and they none of them seem to tell the needed stuff....all cover over stuff not so needed for simple board routing...and cover it over and over.....where are the good videos which tell whats really needed? i can almost recite off by heart the Ferenec and Altium Academy vids, as well as many many others, but am still getting stuck on simple stuff.
Dont get me wrong Ferenec is good....probz the best, but still if you need to just route a simple board its difficult.
Altium wont allow routing
Hi, I am trying to route a track so as to reduce the loop area of the power switching current loop, but altium will not allow me to route in that direction........it just stops, ...it will allow me  to go another direction but that would give poor layout....how do you stop this?.....Tools ...Preferences...PCB Editor.....then what?
Altium is routing things to the wrong place
Altium wont let me route a track to a certain place....it just routes it to a different place, which would give poor layout...how do i stop this?
I seem to have disabled everything in TOOLS PREFERENCES   PCB_EDITOR....but its  still doing it.
I am just trying to do manual routing.
At one point, Altium actually did a "figure of 8" track, going back over itself....that would never ever be wanted....that must be a bug in altium.
This is just a simple 20W flyback board......how do i disable everything so i can just route it up like in Eagle Pro?

[tooki]

1. Reconnect tracks
Hi,
When you move a component and its track comes disconnected, how do you make that track auto-reconnect?
2. Disable everything in Altium
Hi, Am trying to route up a simple PCB...and Altium is making the track dance all over the place as i route it...it wont let me put the track where i want it.......how can i disable absolutely all these extra features in Altium?, so that i can then put them back , individually, as and when  they are required.....for this simple board, i just need Altium to act like Eagle does anyway.
3. Altium videos
Have now watched shedloads of altium videos, and they none of them seem to tell the needed stuff....all cover over stuff not so needed for simple board routing...and cover it over and over.....where are the good videos which tell whats really needed? i can almost recite off by heart the Ferenec and Altium Academy vids, as well as many many others, but am still getting stuck on simple stuff.
Dont get me wrong Ferenec is good....probz the best, but still if you need to just route a simple board its difficult.
4. Altium wont allow routing
Hi, I am trying to route a track so as to reduce the loop area of the power switching current loop, but altium will not allow me to route in that direction........it just stops, ...it will allow me  to go another direction but that would give poor layout....how do you stop this?.....Tools ...Preferences...PCB Editor.....then what?
5. Altium is routing things to the wrong place
Altium wont let me route a track to a certain place....it just routes it to a different place, which would give poor layout...how do i stop this?
I seem to have disabled everything in TOOLS PREFERENCES   PCB_EDITOR....but its  still doing it.
I am just trying to do manual routing.
At one point, Altium actually did a "figure of 8" track, going back over itself....that would never ever be wanted....that must be a bug in altium.
This is just a simple 20W flyback board......how do i disable everything so i can just route it up like in Eagle Pro?

1. There’s a setting for this. While dragging a component (drag, not move!!) press Shift-F1 to list the available shortcuts while dragging. One is the component reconnector.
2, 4, 5. Same thing while placing or dragging a track or component: shift-F1 to see the shortcuts. Among them are the routing style options.
3. I very much doubt you have absorbed everything their videos say. Not a criticism: even understanding everything they say means knowing Altium to a degree that you don’t have yet.

Also, please stop the “make it behave like Eagle” silliness. On the one hand, Altium is not Eagle so it’s unreasonable to expect it to behave the same. On the other hand, many Altium users have never used Eagle, so saying “make it work like Eagle” is completely meaningless to us since we have no idea how Eagle does it. But the best advice I can give for switching to Altium (which is comparatively intuitive compared to many layout programs) is to consciously try and forget what you know about Eagle, and instead approach it as you would if you’d never used a layout program at all. (Ages ago when I worked at the Apple Store, a piece of advice I’d give to people switching from Windows to Mac was “don’t expect it to work like Windows. Instead, forget Windows and just think ‘how would I think it should work?’ and try that.” The customers who did that learned it very quickly; the ones who doggedly expected it to behave like Windows struggled.)

[Faringdon]

Thanks
Updating from library
Hi, i have some resistors , routed in the layout but with keepouts between the SMD pads. The keepout is stopping copper pours on the other side, so i now have to replace all these resistors.
So i got a P&P file showing coords and rotation....then i delete each resistor  from schem, then push this thru to pcb...then replace in schem with resistors with no keepout....then do "properties" on each resistor, and type in coords and rotation.....voila....seems a long way round...is there a quicker way?
Keepouts between SMD pads
How do you do keepouts between SMD pads, such that copper pours are still allowed on the  other side of the pcb to where the resistor is?

[tooki]

In Altium parlance, “updating” a footprint means replacing a footprint with a new version of the same footprint, like if you edit the footprint in your PCB library and want that edit propagated to your PCB. This is done in the footprint editor: in the list of footprints, right-click the footprint and click “update PCBs with (name of footprint)”. If you want to instead change components to a completely different footprint, the best way IMHO is to edit your schematic symbol to add the new footprint, then update the schematic symbols the same way as footprints.

As for the keepouts: I don’t understand why you even think you need keepouts between pads. Just define your clearances correctly, once and for all. If you need different clearances for a specific component, then create a second clearances rule, with some query that will make it apply to the exceptions.

[Faringdon]

Thanks,
Keep getting old "sign in" popup
Hi Altium keeps  freezing very regularly when my old company sign-in popup keeps popping up and inviting me to sign in....but i am already signed in with a different company....do you know how to stop this?....Altium is not useable till ive dealt with the pop-up.

[Faringdon]

How make it NOT "read only"
Hi, i need to change an altium schem and layout, but it just says "read only".....when i go tools ...prefs...Dev Man......etc etc....it doesnt stop it being "read only"...and offers me to save a copy.....when i do that. it deletes all the components when i only delete one....do you know how to solve?
How to stop "sign in" popup keep showing up?
Hi, i am in a "standalone offline" licence, but the "sign in" popup keeps showing up.....when it shows up it stops me from working, till i deal with it...how do i stop it?
Can't modify an Altium pcb/schem
Hi, I have been given an altium project, and need to make changes....but it wont let me...when i delete a component from scm...and push it to pcb, it then deletes all the components from the pcb.
There doesnt seem to be a library within the altium project, and when i go "file....new...library....create integrated library", it produces a title , bit no library...do you know whats going on?...is it some security issue?

[thm_w]

If you can't modify anything maybe your license has become invalid, check the state of that.

I'm assuming this is related to the read only issue, if not check the properties of the file, which should have read-only unchecked.

[Bud]

How to contact your regional Altium Support?

[Faringdon]

Default layer stack region - Default layer stack
Hi, i was just clicking to change all the PCB designators to 1mm....and then must have accidentally clicked something, and now the board has gone kind of all-layers-green, cannot be worked on, and says "Default layer stack region - Default layer stack"....Do you know how to get out of this? [SOLVED...just closed and re-opened]

[tooki]

You pressed “1” while not in any text field, which changes the view to the Board Shape view/editor. (“2” changes to standard 2D view, “3” changes to 3D view.)

[ahbushnell]

Default layer stack region - Default layer stack
Hi, i was just clicking to change all the PCB designators to 1mm....and then must have accidentally clicked something, and now the board has gone kind of all-layers-green, cannot be worked on, and says "Default layer stack region - Default layer stack"....Do you know how to get out of this? [SOLVED...just closed and re-opened]

You should say what you did to make it work. 

[Faringdon]

......Thanks, i just closed the pcb doc and then re-opened it...to make it ok again....it was a bit of a freak fault.....i was pressing "1" regularly to change the text to 1mm....but must have done it "out of sync", and went into the Board shape editor by mistake.
Changing a project name, and the schdoc and pcbdoc name.
Hi, I am doing a new version of a PCB, with the UC2843 chip instead of the LT1243 chip..., so i want to change the project name from "LT1243" to "UC2843", and then start doing the modification.... also wish to change the schdoc and pcbdoc files to be named to "UC2843"  instead of  "LT1243".
Is it ok to do this?......will i loose anything?.....will the design rules , or something, not be there any more?
Also, what about changing the name of the libraries from LT1243 to UC2843?
How to get rid of "Room"
Hi, i have started editing a PCB , to add a few components to it, and a red rectangle, calling itself a "Room" has appeared in the PCB window. How do i get rid of it, is it safe to just delete it?

[tooki]

Nothing was “out of sync”: if you type letters or numbers while inside a text field, you enter text. If you’re not in a text field, keystrokes are processed as shortcuts, and execute commands or settings.

Renaming: do the renaming within Altium by right clicking. But for your application, depending on how big the layout changes will be, you may consider using the Variants feature instead.

Rooms: if you don’t want to use rooms (which aren’t useful in smaller designs IMHO) then you need to disable room generation within the class rules in the Project options. Otherwise the rooms will come back every time you update the PCB. (In one of the most recent updates, Altium changed the project options defaults to not create rooms. But that won’t apply retroactively to projects created in earlier versions.)

[Faringdon]

Thanks,
NetClass_A to NetClass_A clearance?
Hi, if you have a NetClass_A  and you want its nets to be minimum of 3mm clearanced from each other, can you do that in a Clearance Design Rule?........i wondered if it could be difficult, because Altium may try and make the nets clearanced from themselves!?......like.....Net_A must be 0.3mm away from Net_A........Doh!....obviously i   wouldnt  want that.
How to have keepout under SMD component so that copper pour does not go under it?
Please advise?
How to have a courtyard round a component, such that when you push to opposite layer, courtyard goes with it?
Please advise?
Change all circular vias of 0.8D/0.5Hole to 0.6D/0.3hole
.....Do you know how to do this?
How to do auto-routing
Hi,  i have been given a board to gerber up. However, its 4 layer, and the ground plane is so badly cut up that it needs re-doing. Its a micro with loads of connections to lots of opamps, etc, over the board. I believe i will first put in the layer 1 and layer 2 ground planes....then add ground stitching vias near the  chips...then autoroute from there. Is it possible to identify a load of circuitry, and then select it, and then just hit "autoroute, and then it all just happens? Noting that first you have to identify your "preferred" track width for each net, and give the clearance of each net from each other.
Also, we wish the autorouting to be done without going inbetween the pads of an IC or component. (ie no tracks going underneath component bodies)
How to define all vias on PCB as being tented?
...Please advise how?
How to locate all vias of drill diameter 0.6mm?
I can get the "shape" thing that corresponds to them in the drill table...but still finding all 26 of the  0.6mm diameter vias is not easy...do you know a quick way?
Repour shelved vias?
Hi, can you repour vias that are shelved....?....i always get , "repour vias because DRC needs it"....but do i have to then unshelve them, then repour them?...then shelve them again because you cant correct DRC errors with the pours poured.
Component pushing
Hi,
When i am solving clearance errors by pushing components about, sometimes the next  adjacent component starts getting pushed away, before the component that i am moving has got near to it.......there is no collision, but the other component moves away...which is not wanted. How do i stop this? I mean, i have the pusher on...but i dont expect components to get moved before i get near to them. I turned off silk to silk clearance in design rules, but it made no difference.
Vias changed to have 0mm solder mask expansion causes problem
I just made a design rule to make all vias have 0mm solder mask expansion....and Altium must have moved some of the vias nearer to pads, because i am getting minimum solder mask sliver errors which i never got before. Is this a bug in altium.?
Slots in PCB in mechanical layer?
Hi, I put some slots in my PCB using the Altium "SLOT
Change all track widths on PCB?
Hi, just routed a PCB....used many 0.2mm traces....now realise 2oz copper cannot be done with  0.2mm traces without much expense...so now, how do i convert all the 0.2mm traces to 0.25mm traces?
Wont allow error tracks to be moved?
Hi, I have just changed the thickness of all 0.2mm thick traces on layer 2 to be 0.25mm instead. So now there are clearance issues where the tracks are too near to each other.....sometimes it lets me move the track to solve the clearance, but very often it wont let me move it....why wont it let me move it?
Its not as if i am trying to move it into a clearance problem place.
I am speaking of the bits of tracks that are now coloured green as they are clearance error tracks.
...................OK...now it has let me move them.....i just tried moving them from different points, and eventually it let me move them..why is this?

[tooki]

Thanks,
NetClass_A to NetClass_A clearance?
Hi, if you have a NetClass_A  and you want its nets to be minimum of 3mm clearanced from each other, can you do that in a Clearance Design Rule?........i wondered if it could be difficult, because Altium may try and make the nets clearanced from themselves!?......like.....Net_A must be 0.3mm away from Net_A........Doh!....obviously i   wouldnt  want that.

Why don’t you try the solution you propose?

[Faringdon]

Why don’t you try the solution you propose?

Thanks, it seems to have worked, i guess it should have, because the default clearance is "ALL to ALL"

[Faringdon]

Hi,
Doing lib part of a 4 coil common mode choke.
Do you know why i get 4 comon mode choke footprints instead of a single common mode choke with 4 coils?

I have assigned a part of parts A,B,C and D.....ie, the 4 coild of a comm mode choke...but when i place them , itgives me 4 common mode chokes....do you know how to solve?

[Psi]

Hi,
Doing lib part of a 4 coil common mode choke.
Do you know why i get 4 comon mode choke footprints instead of a single common mode choke with 4 coils?

I have assigned a part of parts A,B,C and D.....ie, the 4 coild of a comm mode choke...but when i place them , itgives me 4 common mode chokes....do you know how to solve?

If you only want 1 sch item to place with 4 coils then you shouldn't have assigned parts B, C and D.
You only use the part system when you want multiple placably items within the same component.
Like for a dual/quad opamp where you might want to place each opamp separately on the schematic.
If its just a single item with 4 coils you should only have 1 part and that part has all the pins needed for all your coils.

[T3sl4co1l]

They're either different designators or different UIDs.

Tim

[Faringdon]

Multi Part component
Hi, Thanks,
Now i'm trying to do a dual opamp, MCP6002, one symbol including the power pins. Do you know how to do this?
I can do this easily in Eagle Pro. You just make two symbols separately in the lib...then shovel them both in when you make the "part".

...So now i have got the Part A and Part B in the lib...but it only places one of the parts on the schem sheet.
In the components window, it doesnt show the dual opamp as a 2 part device...but in the schem library, it shows as a 2 part device.

Ive just watched 2 altium videos on how to do this, and none showed how you get the components lib to show the 2 part device.
Even the Altium documentation doesnt show you how to do this....
https://resources.altium.com/p/your-altium-library-multiple-part-symbols-ease-your-design-time

...OK i deleted "U?" then re-typed it and now its ok......i presume i fixed this but it seems a bit bizarre.

..I believe this needs registering as a bug in Altium...i just spent an hour trying to do a dual opamp multi part......it wouldnt work...then it did work when i delted the "U?" designator and then re-typed it , the exact same as it was before i deleted it.

...OK now worked out whats wrong...when you have a multi part..you cannot just click and place, you have to formally go "place part", then right click the multi part, then place it...otherwise you dont get all the multiple parts.......this is not explained anywhere in any Altium documentation or training video. Likewise so many other issues, ...this is why Altium cannot expect to get  bigger sales......admittedly , unfortunately, other than Eagle, Altium is probz the one with best training docs out there. (apart from Eagle , but Eagle isnt as comprehensive) ....but with Altium leaving  problems in like this...it just makes the KICAD bow so much stronger.

Its things like this that prevent people from paying the $10k for Altium plus the $2k per year maintenance....when KICAD is  FREE !!!

[PlainName]

Its things like this that prevent people from paying the $10k for Altium plus the $2k per year maintenance....when KICAD is  FREE !!!

Yep. That's why you're using ... oh, wait...

[thm_w]

Its not an Altium issue, anyway: you place the parts, use shift drag if you want to place the next part in the sequence (eg UxA -> UxB, etc.).
Otherwise you can annotate and it should name them as needed.

https://electronics.stackexchange.com/questions/620773/what-is-the-correct-way-to-use-multi-part-schematic-symbols-in-altium-designer
https://community.element14.com/products/manufacturers/altium/f/forum/10823/annotate-messes-up-multi-part-component

[tooki]

Multi Part component
Hi, Thanks,
Now i'm trying to do a dual opamp, MCP6002, one symbol including the power pins. Do you know how to do this?
I can do this easily in Eagle Pro. You just make two symbols separately in the lib...then shovel them both in when you make the "part".
…

Its things like this that prevent people from paying the $10k for Altium plus the $2k per year maintenance....when KICAD is  FREE !!!

Stop expecting Altium to be Eagle. With that mindset, you WILL struggle, and it’s exactly what we continue to see from you.

The problem when someone expects one program to work identically to another is that they stop thinking about how else one might go about doing it. (Back when I sold Apple stuff, there were tons of people switching from Windows. The people who expected macOS to work just like Windows struggled. I always told switchers “Don’t expect it to work just like Windows. Instead, approach it as though you’d never used a computer at all. How would you intuitively want it to work? That’s how the Mac usually does it.” The switchers who followed my advice mostly did well; the ones who continued to expect it to be Windows found it frustrating.

When I was absolutely new to Altium (and, indeed, EDA software in general) a few years ago, it took me no time at all to figure out how to place multipart components. So it can’t be that hard. It isn’t that hard. Altium is fairly intuitive.

...So now i have got the Part A and Part B in the lib...but it only places one of the parts on the schem sheet.
In the components window, it doesnt show the dual opamp as a 2 part device...but in the schem library, it shows as a 2 part device.

Ive just watched 2 altium videos on how to do this, and none showed how you get the components lib to show the 2 part device.
Even the Altium documentation doesnt show you how to do this....
https://resources.altium.com/p/your-altium-library-multiple-part-symbols-ease-your-design-time

...OK i deleted "U?" then re-typed it and now its ok......i presume i fixed this but it seems a bit bizarre.

..I believe this needs registering as a bug in Altium...i just spent an hour trying to do a dual opamp multi part......it wouldnt work...then it did work when i delted the "U?" designator and then re-typed it , the exact same as it was before i deleted it.

...OK now worked out whats wrong...when you have a multi part..you cannot just click and place, you have to formally go "place part", then right click the multi part, then place it...otherwise you dont get all the multiple parts.......this is not explained anywhere in any Altium documentation or training video.

No, it is documented. You just suck at searching.

https://www.altium.com/documentation/altium-designer/schematic-searching-placing-components says:

Placing a Multi-part Component

If the component being placed has multiple parts, the part selected under the symbol preview image in the Models region of the panel will be initially placed.

Once a part of a multi-part component is placed, it can be changed to another part of this component using the Part drop-down in the Properties panel when the part is selected, or it can be switched to the next available part using Edit » Increment Part Number command from the main menus or the Part Actions » Increment Part Number command from the part's right-click menu.

Likewise so many other issues, ...this is why Altium cannot expect to get  bigger sales......admittedly , unfortunately, other than Eagle, Altium is probz the one with best training docs out there. (apart from Eagle , but Eagle isnt as comprehensive) ....but with Altium leaving  problems in like this...it just makes the KICAD bow so much stronger.

While Altium does have its share of bugs, this is a pure PEBKAC (“problem exists between keyboard and chair”, i.e. user error).

Bigger sales? Altium is already dominant in the low-midrange professional EDA software market, which is why they can hike up their prices as much as they have. You seem to think they’re an underdog or something, struggling for market share? 

KiCAD has essentially zero market penetration in the professional market because it’s just not good enough right now. It does some things really well, but so many others are still just not there*. Can you, with effort, overcome its limitations and produce excellent boards with it? Absolutely! But whereas Altium has gazillions of tools and features to make things go faster**, KiCad makes you do it manually.

But it’ll take a lot more effort than in Altium.

*The fact that in KiCAD it is still impossible to select multiple components and edit them at once (for example, changing the part number of a bunch of resistors) just blows my mind. You have to edit each one individually. Insane.

**Admittedly, perhaps the least-obvious part of the Altium learning curve is learning to configure some of these key tools (most prominently, rules) properly from the beginning, so that the tools are working for you and not against you, as it feels when an incorrectly-configured rule actively blocks something you want to do.

[Faringdon]

Buggy Altiums?
Hi,
Are there certain versions of Altium that are full of bugs?
Because recently i have layed out multiple boards in Altium, 4 layer, with little problem,
and use some of the snazzy features with ease.
At some other companies, i was not able to use their Altium due to constant problems.
(I have used Eagle pro for 20yrs+)
Or i wonder if perhaps a disgruntled staff member can screw up a company's altium?....lace it with bugs?...maybe thats
what happened?

[tooki]

Buggy Altiums?
Hi,
Are there certain versions of Altium that are full of bugs?
Because recently i have layed out multiple boards in Altium, 4 layer, with little problem,
and use some of the snazzy features with ease.
At some other companies, i was not able to use their Altium due to constant problems.
(I have used Eagle pro for 20yrs+)
Or i wonder if perhaps a disgruntled staff member can screw up a company's altium?....lace it with bugs?...maybe thats
what happened?

Excluding actual bugs that cause crashes, etc:

Altium’s behavior behavior is governed by numerous things, including:
- app preferences
- project settings
- rules
- options/modes for the active tool
- grids
- grid snap options
- object type selection options
- layer stack
- impedance profiles
- active layer
- variants
- view options

If any of those is set wrong, it can make it behave in a way contrary to how you want, and it’s easy to perceive this as a bug when in fact it’s working exactly as it should. As one gains experience with Altium, one starts to learn which of these things governs a particular behavior. When set properly, these things all help to enforce one’s particular design requirements.

[Faringdon]

Repeated  un-routed net  issue after design rule check

Hi,
I am running design rule checks, and when i do , certain nodes report "unrouted net" problems.
The track doesnt quite go to the middle of the pad or via.
So then i correct it, and re-run the design rule check, and low and behold, one of the nodes again
has "Unrouted net" problem, and the editted correction that i had just put in has somehow just not happened.
Even though i save the whole project every time that i do a correction.
I am literally just going round and round in circles.
Do you know whats wrong?

(Altium 23)

[tooki]

Sounds like you aren’t actually making the correction you think you’re making. I’ve seen this before, read on:

1. Make sure which rule is actually being violated. You may have unused pins on a component on the schematic, and a rule disallowing this. Place a “generic no ERC” flag (the red x) onto pins which deliberately don’t connect to anything.
2. Make sure the snap settings are correct, and that you’re in the correct layer, so that it’s definitely snapping to the pad center.
3. Make sure that you’re actually looking at the right object! It is possible to end up with little “corpses” (as I like to call them) of traces (or other copper objects) that are hiding out under a pad, so you move a trace, but it’s not actually the offending piece! A few ways to spot these lil zombies:
- use the DRC report to cross-select the offending object
- select the pad
- in the selection filter, turn off everything except traces, arcs, fills, and regions, then do a blue-rectangle select (drag selection rectangle from left to right, which only selects items totally enclosed by the selection rectangle) to enclose the suspect pad area. Delete whatever gets selected.
- hide layers that are obscuring view of the pad area.
- use transparency and/or draft mode settings in View Configuration > View Options to hide or make transparent object types that are obscuring the view

There’s also a really obscure situation involving “free” copper on footprints: before Altium added bona fide custom pad shapes, the way to do them was to draw a fill, then place an ordinary pad onto it. For example, for a weird SMD pad, you’d draw the weird shape as the fill, then place a tiny little no-hole pad on the same layer, right in the middle of the weird shape. When you place and route the component, it’ll assign the weird fill shape the same net as the pad. However, it is possible to inadvertently change this, for example if you cut and paste the component (which, unless you use a Smart  Paste function, removes all net assignments) and the paste location creates net ambiguity, for example if there are more than one vias or traces there. It may ask which one you want to connect, and if you don’t, the weird shape and the actual pad get out of sync. This can lead to unrouted net errors and/or shorted net errors. There’s a menu command that fixes this:  Design>Netlist>Update Free Primitives From Component Pads