Altium Newbie (CS) coming from EAGLE PCB

[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.