Author Topic: Altium questions (Read 16532 times)

PlainName · « **Reply #50 on:** July 21, 2023, 11:10:24 pm »

Quote

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 · « **Reply #51 on:** July 22, 2023, 11:43:56 am »

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 · « **Reply #52 on:** July 22, 2023, 05:14:36 pm »

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 · « **Reply #53 on:** July 22, 2023, 05:37:57 pm »

Quote from: Faringdon on July 22, 2023, 05:14:36 pm

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.

Quote from: Faringdon on July 22, 2023, 05:14:36 pm

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 · « **Reply #54 on:** July 22, 2023, 07:49:19 pm »

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 · « **Reply #55 on:** July 23, 2023, 02:34:39 pm »

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 · « **Reply #56 on:** July 23, 2023, 02:38:30 pm »

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

Faringdon · « **Reply #57 on:** July 23, 2023, 04:50:42 pm »

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 · « **Reply #58 on:** July 23, 2023, 09:00:59 pm »

Quote

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 · « **Reply #59 on:** July 23, 2023, 09:08:11 pm »

Quote

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 · « **Reply #60 on:** July 24, 2023, 08:32:55 pm »

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 · « **Reply #61 on:** July 24, 2023, 08:40:44 pm »

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 · « **Reply #62 on:** July 25, 2023, 03:21:46 am »

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

tooki · « **Reply #63 on:** July 25, 2023, 11:38:32 am »

Quote from: Faringdon on July 24, 2023, 08:32:55 pm

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 · « **Reply #64 on:** July 27, 2023, 08:20:12 am »

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 · « **Reply #65 on:** July 27, 2023, 08:53:50 am »

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 · « **Reply #66 on:** July 27, 2023, 08:55:45 am »

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 · « **Reply #67 on:** July 27, 2023, 09:07:23 am »

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 · « **Reply #68 on:** July 27, 2023, 05:58:40 pm »

I do it like this sometimes.

Tim

asmi · « **Reply #69 on:** July 27, 2023, 08:59:35 pm »

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 · « **Reply #70 on:** August 05, 2023, 08:44:24 pm »

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 · « **Reply #71 on:** August 05, 2023, 09:27:29 pm »

Quote

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 · « **Reply #72 on:** August 05, 2023, 09:45:33 pm »

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

PlainName · « **Reply #73 on:** August 05, 2023, 10:11:57 pm »

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 · « **Reply #74 on:** August 05, 2023, 11:25:05 pm »

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?


EEVblog Main Site	EEVblog on Youtube	EEVblog on Twitter	EEVblog on Facebook	EEVblog on Odysee

Author Topic: Altium questions (Read 16532 times)

Share me