Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Cadstar from the ground up - anyone here can help?

Status
Not open for further replies.

analogNoise

Newbie level 4
Joined
Apr 6, 2010
Messages
7
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,341
I'd like to learn Cadstar, but I'm having some trouble. I'd like to create custom components, my own libraries, etc. I'm investigating Cadstar because it seems that their Signal Integrity integration is pretty good and I'd like to see it in action, but I'm stumped by their library and management. Are there any Cadstar users here who can help?

Thanks!
 

Mattylad

Advanced Member level 3
Joined
Sep 7, 2009
Messages
946
Helped
231
Reputation
464
Reaction score
224
Trophy points
1,323
Location
Lancashire UK.
Activity points
7,220
OH yes....... There certainly is.

What have you looked at so far?
Are you using the CADSTAR Express? it has a good basic tutorial.

CADSTAR is a parts based system, you create a symbol then a component then use a part to join them together.

Are you asking this for personal use or your company? because if the company then there are training courses available.

What version are you using and what are you struggling with?
 

analogNoise

Newbie level 4
Joined
Apr 6, 2010
Messages
7
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,341
Cadstar NSMD.JPG

This is all personal use - I enjoy learning things, and am on a personal quest for a 'better' layout program. I know Orcad/PCB Editor has many high speed design options, but they're so disparate and convoluted that I am trying out Cadstar.

I'm currently creating NSMD pads - I'd like to have a 0.5mm opening and a 0.4mm pad. I have "reassigned" (using Cadstar lingo!) the resist on the top and bottom layers, and set the defaults to the correct pad dimensions. Will this give me a surface mount only pad, or will this create an error where there is a mask opening on the other side of my artwork (don't laugh - I've made that mistake with Orcad Layout, that's why I know to check this!).

I'll keep trying to make my own library components, but some of the items I'm trying to make are relatively high pin-count. Is there an option to import a pin list from an Excel spreadsheet, similar to Orcad? I'd really hate to type out a few hundred pin names.

I'll keep trying (since I seem to have just made some progress) and will ask better questions about it shortly. Thanks for taking the time to help, I hope other people find useful tips here as well!

- - - Updated - - -

For now, it seems I have setup the libraries incorrectly and Cadstar refuses to save the library as I specify due to errors. I have clearly set something up wrong, however I'm on the path to learning. If you've seen this problem and could point me in the right direction I'd be grateful. Thank you!

- - - Update #2 - - -
There is a "Pin File" option if I choose block style symbols. I'll look into this pin format and see how it works and report back, but it looks like what I was looking for to generate symbols for high pin count FPGA style components. So far so good!
 
Last edited:

Mattylad

Advanced Member level 3
Joined
Sep 7, 2009
Messages
946
Helped
231
Reputation
464
Reaction score
224
Trophy points
1,323
Location
Lancashire UK.
Activity points
7,220
Not sure what the N is in front of SMD, as you have defined an SMD pad (no hole in it).
But it looks OK.

You make a pad code, its size/shape etc are the same on all layers unless you reassign them to be something different.

Reassigning or oversizing your solder resist is old hat - its better these days to keep it at 1:1 and allow the manufacturer to adjust it to suit their processes as every manufacturer is different (unless they request you do this).
Reassignments do not swap side when you make an SMD pad and swap the component itself to the bottom, so you need to make the reassignment on both sides in the pad code, you will only see the opening in the solder resist on the side with the pad.

When you add the pad into a component - you choose the side of the board it goes no - Min = top only and make an SMD pad, only ever make SMD components on the min side. IF you add the pad as PTH (but its got no hole) then you see a phantom pad on the bottom layer with no connection - that's because you added it wrongly).

Remember to set your grid to the pin pitch to make adding pads easier, use the interactive origin to set 0,0 so you can put pads at set spacings.

The library editor has a lot of checking in it, you have likely made an error in creating the part so read what its saying when you try to save it as that points to where your going wrong. A snip of the error popup would help to assist you.

And yes it does have a pin list import feature, putting your pin data into an aldec format file works best to enable you to make symbols and part very quickly.
As an example - I can use the wizards to make the component, the symbols and the part for a 484 pin FPGA in about 10 minutes.

That's after I have got the FPGA pin list & modified it in excel, and does not include the cross referencing and checking I do to double check its all correct. (I make mistakes, the vendor makes mistakes - these make the software (any CAD package) make the mistake too.)
So there is no getting away from using a highlighter on printouts to be 100% sure.
 

analogNoise

Newbie level 4
Joined
Apr 6, 2010
Messages
7
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,341
Hi Mattylad,

So I created a pin file in CSV format, but I used the "Legacy input" checkbox and it didn't connect the schematic symbols to the pcb symbol - I think I have to put the "terminal" information in the Graphical Library Editor (GLE). The Aldec format does this automatically, correct?

I tried using the Aldec format, but I didn't get the formatting correct (it failed to import). Do you have an example Aldec format file I could look at? I found the Aldec_pinlist.csv in the SelfTeach folder, but I'm not seeing how I can make sure those schematic symbols/gates match up to the correct pad on the pcb symbol.

This has been tremendously helpful though. I added the items incorrectly to the library, but I saw a Zuken youtube video on how to use "send to" to make sure the symbols were used to create the component, and I was able to use that to send the components to the schematics. It's clunky, but it is working!
 

Mattylad

Advanced Member level 3
Joined
Sep 7, 2009
Messages
946
Helped
231
Reputation
464
Reaction score
224
Trophy points
1,323
Location
Lancashire UK.
Activity points
7,220
Hmm, you have the aldec pinlist file in your self teach - I do not.

Are you using the Express version?

The aldec pinlist should be a good enough example, it does enable you to make a multigate file while using the symbol wizard.
Then when making the part you select the component, add the symbol gates that are the symbols you made in the wizard then on the pins page - load the multigate file and it auto allocates the symbol pins.

Have you made a part without using a pinlist? You need to learn to do this before using the more advanced pinlist setup so that you understand what its doing.
 

analogNoise

Newbie level 4
Joined
Apr 6, 2010
Messages
7
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,341
I had a trial of the full Cadstar, and I requested the supporting files for evaluation. Now I'm on the express version - I wasn't able to convince my work on what I could teach myself that it was better than Orcad (which everyone uses, but nobody uses well).

I'll make parts without the pinlist as you suggested to get the necessary skills. Thanks again Mattylad!
 

Mattylad

Advanced Member level 3
Joined
Sep 7, 2009
Messages
946
Helped
231
Reputation
464
Reaction score
224
Trophy points
1,323
Location
Lancashire UK.
Activity points
7,220
That's the problem, everyone uses orcad but not well, just like many also use CADSTAR - but not well.

I am seeing people who have used it for years who do not know some of the basics when I train them and their colleagues.
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top