Altium Newbie (CS) coming from EAGLE PCB

[IanJ]

Hi all,

Carl at Farnell said to me on the phone.........you'll get into situations where you can't find stuff, or don't know how to do this or that.....but keep looking it's there, and can be done.

With that I installed CS and as a complete an utter Altium newbie I started playing, but on my i5 laptop, not my Dev PC (which I'm rebuilding) so screen res is hindered to 1366*768, and just one monitor.................ach I thought I'd give it a go!
The target - to convert one of my existing Eagle PCB designs to CS.......same schematic layout, same designators, same exact PCB layout and hopefully track layout.

Some components from the vault, some from the built in library, and one or two from VinceH's (kindly publsihed online). There's also about 6 components I've had to design from scratch myself.

You know, moving from EaglePCB it's not that bad.......once you get your head around how the schematic and footprint parts of the libraries work in comparison to Eagle.

There's a few bugs, issues, crashes, memory leaks, and missing functionality in CS, mostly to do with the vault/libraries......but I'll detail those later. I'm making notes along the way. And, just like any other design there's moments where you have to walk away and come back.

I'm about 3 days in........and the following screenshots I think show I am making progress......and as you'll see I haven't started routing yet so I don't know whats in store!

PS. No cheating, the Eagle import function is NOT being used.......:-)

Ian.

[rx8pilot]

As an Eagle user - this is exciting to watch. My biggest concern moving to Altium would be the challenge of the learning curve.

Look forward to seeing this play out.

[LabSpokane]

How are your user-created components doing?  I can't get any of mine to be placed properly on the PCB. 

[EEVblog]

With that I installed CS and as a complete an utter Altium newbie I started playing, but on my i5 laptop, not my Dev PC (which I'm rebuilding) so screen res is hindered to 1366*768, and just one monitor.................ach I thought I'd give it a go!

Yep, Altium (Designer or CS, same thing) is painful on a single screen, let alone 1366x768
IIRC there are even some dialog boxes at that screen res that are not usable.

[EEVblog]

As an Eagle user - this is exciting to watch. My biggest concern moving to Altium would be the challenge of the learning curve.
Look forward to seeing this play out.

Me too.
It will be interesting to see how hard it is for Eagle users to switch.

[IanJ]

How are your user-created components doing?  I can't get any of mine to be placed properly on the PCB.

I had same problem.......compiled ok, updated PCB and all components went across EXCEPT my user created ones. Not sure exactly what I did but I jumped around checking everything from the adding of the footprint to the schematic, to compiling everything and saving, and restarting the app.......then when I updated the PCB again my new part was suddenly there.
Whether I did something wrong or there's a bug I don't know.
I have some other components still to sort out so will try and see exactly where it or I is falling over.......but I've a feeling the restart did it.

Ian.

[IanJ]

With that I installed CS and as a complete an utter Altium newbie I started playing, but on my i5 laptop, not my Dev PC (which I'm rebuilding) so screen res is hindered to 1366*768, and just one monitor.................ach I thought I'd give it a go!

Yep, Altium (Designer or CS, same thing) is painful on a single screen, let alone 1366x768
IIRC there are even some dialog boxes at that screen res that are not usable.

So far there's only one dialog box I came across where the OK & CANCEL button are inaccessible right smack under the task bar.........had to use TAB to reach 'OK'.

Ian.

[IanJ]

Does it support shotcuts? Such as PL for placing wire, PT for placing track (wire with net), PV for placing via, etc.?

List:
http://documentation.circuitstudio.com/display/CSTU/HelpAdvisor_Pnl-Shortcuts((Shortcuts))_CS

Ian.

[tautech]

Nice going Ian, have you figured out all the hidden pop outs on the side bar, I see you have the file structure one out all the time. 

[LabSpokane]

How are your user-created components doing?  I can't get any of mine to be placed properly on the PCB.

I had same problem.......compiled ok, updated PCB and all components went across EXCEPT my user created ones. Not sure exactly what I did but I jumped around checking everything from the adding of the footprint to the schematic, to compiling everything and saving, and restarting the app.......then when I updated the PCB again my new part was suddenly there.
Whether I did something wrong or there's a bug I don't know.
I have some other components still to sort out so will try and see exactly where it or I is falling over.......but I've a feeling the restart did it.

Ian.

It's finally working for me.  Albeit, on a different computer that has never had CircuitMaker installed.

My new problem is that I keep getting "pin not found" errors when validating and executing a part addition to load new parts onto the PCB.  Many times, I'll get errors, but if I execute, the part ends up on the PCB with the correct air wires.  There's a few windows that have the text clipped.  The pin editor suffers from this. 

[LabSpokane]

As an Eagle user - this is exciting to watch. My biggest concern moving to Altium would be the challenge of the learning curve.
Look forward to seeing this play out.

Me too.
It will be interesting to see how hard it is for Eagle users to switch.

There is a very low learning curve switching from Eagle. Almost all of the issues that I am experiencing are related to the Vault accessibility and user component generation.  If Altium would actually respond to my inquiries and find a workaround/fix or give me the secret knock, it would be a no-brainer purchase. 

I just got an email from E14/Altium today with links to several tutorial videos - one of which was on part creation.  I thought I was saved.  I would discover the errors in my ways.  Sadly, it turns our that Altium's video doesn't show the user the correct /complete way to create a part.  They left out the key step of how to link the schematic to the footprint.   

[rx8pilot]

There is a very low learning curve switching from Eagle. Almost all of the issues that I am experiencing are related to the Vault accessibility and user component generation.  If Altium would actually respond to my inquiries and find a workaround/fix or give me the secret knock, it would be a no-brainer purchase. 

Overall, that sounds encouraging. I suspect the user components challenge is primarily an education/documentation issue? Even if you know every trick in the book - creating parts in Eagle is about as fun as lemon juice in your eyes.

[LabSpokane]

There is a very low learning curve switching from Eagle. Almost all of the issues that I am experiencing are related to the Vault accessibility and user component generation.  If Altium would actually respond to my inquiries and find a workaround/fix or give me the secret knock, it would be a no-brainer purchase. 

Overall, that sounds encouraging. I suspect the user components challenge is primarily an education/documentation issue? Even if you know every trick in the book - creating parts in Eagle is about as fun as lemon juice in your eyes.

Which brings us to CS documentation: there is very little available, and nothing covers the nuances that would resolve my problems. Today is day six of waiting for a response from Altium on a laundry list of issues. I'd nearly settle for a RTFM manual response because then, at least there would be a FM.

I'm not giving up quite yet because this really is the Promised Land of powerful tools for the prole. But, I'm starting to get a taste of Altium's notorious dysfunctionality. 

This weekend I'm going to install a trial of Designer. It will be a good test. If the problems follow, it's user error. If they go away its software error.

I'm really hoping its me because that means I can learn the trick and be off and running.

[IanJ]

It's finally working for me.  Albeit, on a different computer that has never had CircuitMaker installed.

My new problem is that I keep getting "pin not found" errors when validating and executing a part addition to load new parts onto the PCB.  Many times, I'll get errors, but if I execute, the part ends up on the PCB with the correct air wires.  There's a few windows that have the text clipped.  The pin editor suffers from this.

Well, for the life of me I couldn't get a 2nd custom part onto my PCB. After Execute the ECO reports unknown pins.........but everything is in place!

So then I deleted the footprint reference (Model) under EDIT in the Schematic library.......and re-attached it, but specifically I added it again by selecting LIBRARY PATH and navigating manually to the lib it's in. At that point the bottom window will say can't find.......but then type in the NAME of the component under NAME at the top, your footprint image should appear in the box.
Update schematic, compile etc then when I then updated the PCB......BINGO!

So what I believe is that there's only a specific way you can attach your footprint that works, even though either of the ways to reference the library it's in appears to work.

It's either that or it was another fluke!

I have more to add to the pcb........so I hope it's repeatable.

Ian.

[LabSpokane]

It's finally working for me.  Albeit, on a different computer that has never had CircuitMaker installed.

My new problem is that I keep getting "pin not found" errors when validating and executing a part addition to load new parts onto the PCB.  Many times, I'll get errors, but if I execute, the part ends up on the PCB with the correct air wires.  There's a few windows that have the text clipped.  The pin editor suffers from this.

Well, for the life of me I couldn't get a 2nd custom part onto my PCB. After Execute the ECO reports unknown pins.........but everything is in place!

So then I deleted the footprint reference (Model) under EDIT in the Schematic library.......and re-attached it, but specifically I added it again by selecting LIBRARY PATH and navigating manually to the lib it's in. At that point the bottom window will say can't find.......but then type in the name of the component under NAME at the top.
When I then updated the PCB......BINGO!

So what I believe is that there's only a specific way you can attach your footprint that works, even though either of the ways to reference the library it's in appears to work.

It's either that ot it was another fluke!

I have more to add to the pcb........so I hope it's repeatable.

Ian.

That's the exact error I'm getting. Will try your trick. Thanks for sharing!

[IanJ]

That's the exact error I'm getting. Will try your trick. Thanks for sharing!

Just tried again and appeared to work first time for me.

PS. Have edited my post a couple back just to make it clearer.

Ian.

UPDATE:
Yes, very repeatable, just added 4 more custom components first time.
There is an issue with using a custom schematic component and a library footprint, dialogue says footprint not found (but it is ok), and when updating the PCB a pop-up complains about possible NET issues, but all goes through ok.

The biggest positive with all this, and CS in general is that you can change between schem editing, footprint editing, the main schematic/pcb etc etc etc without leaving any of the processes, they are just tabs on the robbon.............a HUGE positive over EAGLE PCB.

[IanJ]

Nice going Ian, have you figured out all the hidden pop outs on the side bar, I see you have the file structure one out all the time. 

Just that one and the PCB/SCH LIBRARY editing ones.

Ian.

[IanJ]

Wow......this makes a change from Eagle!

Ian.

[LabSpokane]

The solid model is pure gold. 

I haven't gone much farther than the errors that I've been flagged with, but I may see if I can drive a test design all the way through OSHPARK and see what happens.

[LabSpokane]

The biggest positive with all this, and CS in general is that you can change between schem editing, footprint editing, the main schematic/pcb etc etc etc without leaving any of the processes, they are just tabs on the robbon.............a HUGE positive over EAGLE PCB.

Part creation workflow and management in CS is a massive improvement. Once we have the little bugs worked around, there will be no comparison.

=======

Ian,

Have you tried attaching STEP files to parts yet? 

[rx8pilot]

Part creation workflow and management in CS is a massive improvement. Once we have the little bugs worked around, there will be no comparison.

Fantastic news! Thanks for the play-by-play.

I found myself avoiding improvements in my designs because it is such a penalty to add new parts. If creating new parts is reasonably easy and quick - I am now paying much closer attention to this option. Much closer.

[IanJ]

Hi all,

Am I having a senior moment!............is it not possible to copy symbols or footprints from the vault or any of the built in libraries? I simply want to duplicate and then edit a 3.2mmx1.6mm tant cap footprint to make a slightly bigger one.........rather than draw from complete scratch?

Related......I came across a new issue today, I used the schematic symbol from one lib and a footprint for from another and got the unrouted pin error when dropping it onto the PCB............just had to edit the pins as they didn't match. Job done, but I'd also like to be able to save my fixed component to my own wee library.......but how?

#####

LabSpokane,
No haven't look at the step files at all yet.........won't be looking at that till I get this pcb fully routed and optimized.

Ian.

UPDATE:
The new component wizard goes some way to helping.......at least there isn't the need to manually create pads etc when creating a new footprint. Still, the ability to copy and paste symbols etc from the library has to be included.
Also, if a package is locked (i.e. an Altium library/vault component) then the ability to ADD a secondary footprint would be good to have. At the moment it seems like the user is locked out completely.

[LabSpokane]

Part creation workflow and management in CS is a massive improvement. Once we have the little bugs worked around, there will be no comparison.

Fantastic news! Thanks for the play-by-play.

I found myself avoiding improvements in my designs because it is such a penalty to add new parts. If creating new parts is reasonably easy and quick - I am now paying much closer attention to this option. Much closer.

I'm seven days and counting with no response from Altium, so I'm questioning their commitment to Sparkle Magic. Even so, we will win if and when Autodesk reinvents Eagle. CS is sooo close to being ready for prime time that it could really be a horse race.

[LabSpokane]

Hi all,

Am I having a senior moment!............is it not possible to copy symbols or footprints from the vault or any of the built in libraries? I simply want to duplicate and then edit a 3.2mmx1.6mm tant cap footprint to make a slightly bigger one.........rather than draw from complete scratch?

Related......I came across a new issue today, I used the schematic symbol from one lib and a footprint for from another and got the unrouted pin error when dropping it onto the PCB............just had to edit the pins as they didn't match. Job done, but I'd also like to be able to save my fixed component to my own wee library.......but how?

#####

LabSpokane,
No haven't look at the step files at all yet.........won't be looking at that till I get this pcb fully routed and optimized.

Ian.

Ian,

The vault and supplied libraries are locked down. That was one of my major complaints to Altium. I'll post their response as soon as I get one.

[tautech]

Hi all,

Am I having a senior moment!............is it not possible to copy symbols or footprints from the vault or any of the built in libraries? I simply want to duplicate and then edit a 3.2mmx1.6mm tant cap footprint to make a slightly bigger one.........rather than draw from complete scratch?

Related......I came across a new issue today, I used the schematic symbol from one lib and a footprint for from another and got the unrouted pin error when dropping it onto the PCB............just had to edit the pins as they didn't match. Job done, but I'd also like to be able to save my fixed component to my own wee library.......but how?

Fully fledged Altium allows creation of a Project library, can you not do that?

[bson]

Am I correct in that CS doesn't support non-round holes (like required for many micro USB connectors) - but I assume it can do milled cutouts?  It's there a minimum size for millouts in CS? Also, does it have push-and-shove routing?

[LabSpokane]

Am I correct in that CS doesn't support non-round holes (like required for many micro USB connectors) - but I assume it can do milled cutouts?  It's there a minimum size for millouts in CS? Also, does it have push-and-shove routing?

It has multi routing and differential pair routing. I have not figured out how to use either yet, but they exist in the menus. The routing is head and shoulders above Eagle. Most will enjoy it. Very easy to route neat tracks with clean, 45 deg angles.

Slotted holes both played and unplated are supported.

Cutouts are easy and supported. 

[rx8pilot]

I am warming up my credit card already. Not interested in waiting for the possibility that Eagle will be saved by Autodesk. 

Sent from my horrible mobile....

[LabSpokane]

I am warming up my credit card already. Not interested in waiting for the possibility that Eagle will be saved by Autodesk. 

Sent from my horrible mobile....

Wait for a response from Altium on the part creation. You won't want to fight that for long and not for 50 Tubmans.

[IanJ]

UPDATE:

Got my PCB component layout all sorted, exacted all critical positions and approxiamated everything else. Routing was of course my next big hurdle, but put my faith in Altium being top notch and so far it's working out great. Just have to remember all the shortcuts.

Here's a few screenshots.......2 from CS, 1 3D view from AutoTrax DEX (don't ask!), and the last my source layout from EAGLE.

CS - Work-in-progress:


CS - 3D view:


Autotrax DEX - Iliya, if you read this: The GUI is fast and yes you can drop via's down onto a copper pour and the NET is completed:


Eagle PCB - my original layout:

[IanJ]

Hi all,

Been playing with SNAP, GRID and GUIDES.

In EAGLE if your primary GRID is 25mils you can set a secondary grid to anything you like, and it's handy to set it to half of the primary i.e. 12.5mils. Accessible by holding down ALT as you move or place stuff around. Real handy if you have a mix of MILS and MM components.

Is there an equivalent in CS?

Ian.

[LabSpokane]

Ian,

I've been hoping for the same grid spacing tool in CS. It should be there, but I'm still trying to find it.

Good job on the layout!  Isn't routing in Altium's fun compared to Eagle?  I love it.

[tautech]

Ian,

I've been hoping for the same grid spacing tool in CS. It should be there, but I'm still trying to find it.

Good job on the layout!  Isn't routing in Altium's fun compared to Eagle?  I love it.

In Altium it's in the Project tab and within a popup on the bottom bar.

[IanJ]

Looks like apart from the inteligent object snap etc that CS has the only way to change the snap grid is to right click and select one of the presets (or type a custom one in).........CTRL G or SHIFT CTRL G are the shortcuts. Hmmm, a tiny bit clunkier compared to Eagle as I must say I made LOTS of use of the ALT function in Eagle.
An additional shortcut key to disable snap would be great also, albeit you can enter zero under SHIFT CTRL G.

Wishlist items I think.

If this is not possible then at the very least have the SET SNAP GRID custom entry remember what it was set to previously. At the moment when you re-enter that menu it picks up what the main snap was set to.
I.E. if you start at a fixed 25mils, go to a custom 12.5, then back to a fixed 25 then when you go back into the custom it picks up 25..........would be slightly better if it remembered the previous custom of 12.5.

Ian.

[IanJ]

Hi all,

I've got DRAG working with, i.e. move a component AND the connected traces........something I used in Eagle so looking to reproduce it easily in CS.

Is there a shortcut key for this....can't find.

I read AD supports CTRL and drag the component but that doesn't work with CS........the traces just stay behind.

Ian.

[LabSpokane]

Ian,

Try this:

Recompile the schematic then right click on the bare PCB and there should be a routing preferences panel.  That fixed that for me. I got very workable push/shove routing as well from altering the config.

[IanJ]

Ian,

Try this:

Recompile the schematic then right click on the bare PCB and there should be a routing preferences panel.  That fixed that for me. I got very workable push/shove routing as well from altering the config.

Yup, I got it working......I just need a keyboard shortcut for it. In AD you can edit shortcuts, but looks disabled in CS.

PS. I quite like the HUGNPUSH obstacle mode.

Ian.

[IanJ]

99% finished CS versus Eagle. I have changed CS colours to match my colours in Eagle - don't ask, this goes way back to my use of Wintek's Smartwork/HiwireII.

I have sent the CS gerbers off to Elecrow (my usual pcb maker) for evaluation and to check my workflow as there are some unique things in the CS gerbers like slotted plated holes, certain via's tented only and to check the solder/copper mask is ok and that the board outline (or lack of it) is ok.

Ian.

[tautech]

There's a few different TH annular rings, pad and hole sizes, was that intentional?
Or a trick in the imagery?

[IanJ]

There's a few different TH annular rings, pad and hole sizes, was that intentional?
Or a trick in the imagery?

Intentional, albeit I haven't fully checked yet.
The slightly larger via's are to GND, the rest are signal.
The holes sizes on the PCB switch had huge holes (from the library) so I just changed them on the fly.

Some of the SO8 packages are wrong (possibly CS bug I am exploring).

Ian.

[LabSpokane]

That's fantastic Ian. 

Have you had any problems with getting "Please wait" messages and system crashes?

[IanJ]

Have you had any problems with getting "Please wait" messages and system crashes?

Yes I have, a couple times a session usually. The PLEASE WAIT messages with the progress bar that repeats itself and eventually ends up in an error message. I have reported it.

Ian.

[Morgoroth]

Hi all, I'm jumping on this thread to ask if someone knows clearly the limits of Circuit Studio and 3D models integration, I want to buy an Altium Designer licence but seems Circuit Studio is very close to my needs and far cheaper.

I have to work with a mechanical engineer that use SolidWorks and a designer that use Maya, and the only one thing I'll miss will be the very handy PCB filter.

Thanks in advance,

 JP

[LabSpokane]

Hi all, I'm jumping on this thread to ask if someone knows clearly the limits of Circuit Studio and 3D models integration, I want to buy an Altium Designer licence but seems Circuit Studio is very close to my needs and far cheaper.

I have to work with a mechanical engineer that use SolidWorks and a designer that use Maya, and the only one thing I'll miss will be the very handy PCB filter.

Thanks in advance,

 JP

Ian has had more success than I (and has more talent) and I'm sure will have a different opinion.

Personally, I will work around some peccadilloes, but when it comes to the frequent system hangs and crashes, I have to draw the line.   I would not buy CS as it stands today as a substitute for AD, particularly if the consequence of being delayed on a design cost me more than $5000 USD.  CS simply has *zero* support.  If you can't find a canned answer somewhere, the answer will not be coming from E14/Newark, and it sure as hell won't be coming from Altium.  Element14's support consists of taking your email and forwarding to Altium (to evidently be ignored).  Buy AD, and you'll get immediate support and full documentation.  Buy CS, there will be virtually *no* documentation save for a couple of tutorials, some of which are demonstrably wrong/incomplete.  Get stuck with CS, and you're stuck for good and without $1000. 

If CS 1.2 was a beta release, I'd be doing cartwheels.  But it isn't.  It's been in the market for years and has major, in my opinion, showstopper flaws that preclude one from taking it seriously.  And that is sad, because what is working is simply brilliant.

[IanJ]

Hi,

I don't know about 3D integration, very early for me......I've only been using CS for 10-days, prior to that I'd never used any of Altium's products at all, only EAGLE PCB for the past 4 or 5 years.

V1.2 is close, very close. I have been in direct contact these 10-days with Altium and have been forwarding to a contact there the bugs, issues and feature requests I have come across. I don't know what/when the reaction will be......but from what they tell me they seem to be very active with it (developing & marketing etc). It's all quite positive right now.

Latest from me:
I have been working with Elecrow to get the gerber workflow sorted. There's a few Altium quirks and default settings I wasn't aware of that need changed hence a couple emails back and forward with Elecrow. I chose Elecrow because I have been using them with EAGLE for years, and they support slotted, plated holes etc (unlike Oshpark I believe).

Ian.

[IanJ]

Hi all,

Elecrow compatible 2-layer, SMD/TH gerber files.
Took me two attempts at sending a ZIP to Elecrow till they confirmed the gerbers were fine. They sent back screenshots to me to confirm.
The only issue I had with the original default gerber settings was that I was getting lots of extra lines etc on every layer. The right hand pane on the layers tab was to blame. See below.

PREPARATION:

On the OUTLINE layer draw a line around the edge of your board to match Altium's board limits. Not sure if Elecrow actually need this, but I happened to have it on because OSHPARK needed it.
The settings below probably more than cover a 2-layer board etc, but this is just what I had mostly from defaults.

GERBER:

General tab:
- Units = Inches
- Format = 2:4

Layers Tab:
- Select GTO, GTP, GTS, GTL, GBL, GBS, GBP, GBO only
- In right hand pane de-select all 5.
- Bottom pane select Include unconnected mid-layer pads

Drill Drawing Tab:
- Drill Drawing Plots - select Bottom Layer-Top Layer
- Drill Guide Plots - select Bottom Layer-Top Layer

Apertures Tab:
- Select Embedded apertures (RS274X)

Advanced Tab:
- Film size X=20000mil, Y=16000mil, B=1000mil
- Aperture Matching Tolerances Plus=0.004mil, Minus=0.004mil
- Batch Mode = select Separate file per layer
- Leading/Trailing zero = Keep
- Position on Film = Ref to absolute
- Plotter type = Unsorted
- Other - select Optimize change & Generate DRC rules

NC Drill Setup:

- Units = Inches
- Format = 2:4
- Leading/Trailing zero = Keep
- Position on Film = Ref to absolute

Any checkboxes not detailed above leave un-checked.

Hit the GERBER button then once it's finished, hit the NC DRILL FILES button. Under your project in a folder starting "Project Outputs for........" will be a host of files. ZIP up the files starting with "PCB1" only and thats it.

Ian.