Export CAD Data From CAM350 to PowerPCB?

[nina]

Hi there,
I'm trying to get an 'export CAD data' function to work. The ultimate goal is to translate an Allegro layout to a PowerPCB layout. I thought I could do this by:
a) getting Allegro gerber files
b) import the gerber files into CAM350
c) export from CAM350
d) import the resulting .asc file into PowerPCB

When I try File > Export > CAD data, all the radio buttons for the various output formats (including PADS) are greyed out. Under Access Code, we have the access code typed in (hardlock), and Export is checked as one of the features we have with this Access Code.

Any ideas why PADS is greyed out?

I should note that we will be making mods in PowerPCB eventually.

TIA!

nina

[Skip Yutkus]

Don't know why your export buttons don't work, you'll need to talk to Downstream about that, but what you describe as your goal and the method you plan to use seem to be a little too simple, unless you plan on rebuilding all of the components in Cam350 then the ascii information will be of very little use, you will not have any decals or nets, just dots and lines. Even if you rebuild the components the net names will be gibberish. A better solution would probably be the RSI translator.

Skip

[nina]

Hi Skip,

I should clarify - I'm assuming that once I import into PowerPCB it will simply be a graphical representation. I will then have to take a netlist from Allegro (actually I will be taking it from OrCAD Capture, I've got that working) and 'reproduce' the layout using the netlist, x-y coordinates, and the graphical representation. I did take a look at places like ratpack.com and rsi-inc.com. I don't know that I'd save any time going through them, plus of course the $$ and NDAs to worry about. I was going to send them a request for info though - what is their final output, do you know? I guess I have to send them our part and decal library?

nina

[Skip Yutkus]

RSI translates just about any format to any other format in use today - but keep in mind translation is never perfect you always have to reconstruct some of the data, I think that you pay based on how many formats you want to translate, it also occurs to me that when you do it either way, the layers might end up on the wrong layers in pads, this I don't know, I don't have the RSI translator and currently we're using BoardStation. Another solution is to have RSI translate your data, I think they offer this service.


Skip

[nina]

This is pretty much a one-time thing so probably we'd be more interested in paying them to do the translation rather than buying the software. I should probably send them an e-mail for details.
Regarding the CAM350 I'm not sure I will get tech support since our license has recently expired. Guess it can't hurt to try.
Thanks for your input.

[randychase]

nina, we might be able to help you since we have done some CAM-350 gerber to PADS translations.

[nina]

Hi Randy,
Actually, I did try to visit your website but didn't get anywhere...? What exactly do you mean by translation? Is there company-specific part decal and part name information in the final result? Once we have a .pcb file, we plan to recreate the schematic from it in PowerLogic, so that we have a fully synchronizing version of this board. We will need to make modifications to this board down the road; that's why we need more than simple gerber files. I'm currently mapping the Allegro BOM to our PowerPCB part names. I don't know yet how different our land patterns are though (don't have the Allegro file yet).

nina

[randychase]

By translation I mean, you can take the gerber files into CAM-350, and with some effort, you can create a PADS file, as you first attempted to do. It's a little tricky, you have to extract a netlist and build components. And even then you might end up with some oddities that will require you to design over with new parts and traces.

Anyways, I am saying if you need it translated from CAM-350 to PADS, my company can do it, as can others.

Next question, how complicated is the board? Number of layers? Planes? Simple or mixed planes? Size of board? Number of parts?

[nina]

Let's see... I actually don't know too much about the board yet, as I don't have the file. The only things I know are the size (5" x 7"), and 6 layers. I don't know the plane structure, whether or not there are blind/buried vias, etc. There are 432 components, approximately 350 of which are res/caps.
I have discovered a few companies that do the translation services; I guess I need to figure out which company would best suit our needs, or if we'll just do it ourselves, but (naturally) we do have time constraints to consider.
Randy, to what extent does your company complete the translation - can the .pcb file synchronize to a PowerLogic schematic? I guess I don't really know how our own PowerPCB libraries get incorporated into the file. I'm assuming that it is a 'simple' mapping of the Allegro parts to our PowerPCB parts and decals. Sorry if the answers to my questions are obvious, I really don't know much about what a translation service entails.
Thanks.

[randychase]

This is a general answer to how it works.

In CAM-350, you group an item into a part and call it a part. Doesn't matter too much what you call it. But you need to define that the 16 pin part is an SO-16 and that the 2 pin part is an 0805 for example. You play with layers some. Then you extract the netlist and create the database.

The database is read into PADS and you can then replace the parts using the ECO mode with your standard library parts. That is how I have done it. I don't like the library parts created from the translation. It's pretty easy to do, as you can do it globally to all 0805s for example.

You can tweak the design and your schematic to get them to sync up.

One other option you should not overlook, is making a new design using the old one as a template. For some reason, I end up doing this a lot. With a good schematic and a board in hand, it's pretty simple. When I do it for the military, they require that all the traces look the same. Now that is more difficult. :)

[H.Tikkanen]

Even if you decide to redo the design, it makes sense to use CAM350. It is very easy to set up layers, run draw to flash conversion, and export to PowerPCB. If you haven't built the parts, every pad appears as a single component. Traces appear as 2d-lines. They can be moved to a documentation layer, and you can use them as a quide to reroute the real traces.

Also, a BOM can be easily modified to PADS format and read in by ascii import. Works well if parttype names match. Just check the rotation and placement of decals with non-origin centers.
-hannu tikkanen-

[Boarddesigner]

Hello Nina,
The process for re-generating pcb data from gerber data can be complex and is usaully more economically feasable when left to the pros. Such as Randy Chase.
But if your into taking on an entire learning curve, then by all means have at it.
Here is the process in a nutshell:

1. load gerber data in cam350, including drill data.
2. Assign the appropriate layers: top silk, top layer, etc.
It will be cleaner and faster to not have fab notes, assembly, mechanical, etc.. loaded in design
3. Align all layers top, bottom, ncdrill, etc..
4. Convert draws to flash
You can convert positive plane data as well. But if you have alot of plane area this might slow done the process. (a 5x7 board should be ok)
5. convert pads to padstacks
6. create parts
The best way to do this is to use the build part rather then quick part. Also, if you have an existing schematic make sure to name your parts exactly as they are in the schematic.
7. Load original netlist
Having the original netlist is very helpful in verifying that all the previous steps have been done correctly. (incorrect pinouts, reference designators, etc.)
8. If there is no original netlist to reference to then the next step is to create a netlist from gerber data. At this point you are now ready to export usable cad data.

>>Note:
It has been a couple of months since I last converted a design and might have unintentionally excluded a detail or Two.
All the same the above process should be helpful as a general guide. <<

Good luck and
haveagoodone

Boarddesigner

[nina]

Dear all,
Thanks much for your advice - I've got a better idea now of what is involved in the process. Seems my original thought of using the CAM350 output as a template (that was the word I was looking for!) will work, but perhaps the result will be more accurate if I follow those steps outlined above. Although, as you say, it will involve somewhat of a learning curve (which surprise surprise we probably don't have much time for).
Again, thanks everyone for your help in this.
Randy, how would I go about getting a rough quote from you, just to keep my options open?
Thanks,
nina

[nina]

Hello again,
Is there anywhere I can get docs on CAM350? I would like to do a simple export from gerber data to CAD data (PowerPCB), but I don't know the process (in fact I've never used CAM350). I can import the gerbers fine, everything is aligned, but don't know what else is involved in setting up layers. I tried running the Utilities --> Draws-to-Flash --> Automatic, but I know I'm still missing some steps. When I go to File --> Export --> CAD Data, everything is greyed out. I'm not sure if this is because I'm missing some steps, or because there's something wrong with the license (hardlock license, expired a couple months ago). I'm going to also try contacting Downstream but since our license has expired not sure if that will help.
Thanks,
nina

[randychase]

The help file is pretty clear on the steps required to do a conversion.

I think the policy at Downstream is to allow you one free phone call after you are off maintenance.

For some reason, my key expired before and I had to call to get it working.

[randychase]

As far as having it done outside, if you want me to look at it, email me the zipped gerbers.

[nina]

Thanks Randy,
I didn't know that about Downstream.
In fact, I don't have any gerbers yet (I'm just experimenting on one of our own gerbers). What is your policy on NDAs?
nina

[thienthu]

Hi Nina,

It's been 6years from your post here and now I want to do the same thing. Could you tell me if you succeed or not? Do you have any suggestion about this translation/convertion?

Thank you very much.
TT