Problems exporting ODB++ files and P-CAD ASCII file

Report bugs here
Message
Author
eosrisko
Posts: 10
Joined: 04 May 2016, 10:16

Problems exporting ODB++ files and P-CAD ASCII file

#1 Post by eosrisko » 05 Mar 2018, 09:17

Hello guys,


What I will report I had already asked the question in another post posted by another member. But as I just checked another problem, I decided to create a post for it.

I am currently doing a PCI project for a board manufacturing company and as I am changing the project I export the ODB ++ files for analysis in the company's software. They use very conservative boundary rules and I have to change the Solder/Paste Mask (decreasing the size of the paste on the pads that will receive solder) to each analysis response.
To change the Solder/Paste Mask rule only for the specific component pads that reported error in the company software scan, I did the following:


And I changed the following options, highlighted in the image below:


As a result of these changes, I generated the Gerber and opened the Top Mask to check the Paste spacing between the component pads:


So far, all right! I generated the ODB ++ files for the company to analyze ...

But, the company is having difficulty opening my ODB++ files exported by Diptrace. In the software they use for analysis (I do not know what it is) returns this error:




For them to analyze my project I have to export to P-CAD ASCII and then they open this file in Altium software and export to ODB++. Why are they not able to open the ODB ++ exported by Diptrace. Do you have any ideas that can help me?

These were the first questions. Continuing ...

As the company can not open my ODB ++ files. It uses my P-CAD ASCII file doing the conversion to ODB ++ as I reported above. However, I did open the errors reported by the most current analysis they sent me, and I noticed that the changes I made in the Solder/Paste Mask to the pads of the specific components were not exported together with the P-CAD ASCII. What I thought was that only the rule set as default in Diptrace was exported, whereas my specific changes were not. The result of the company analysis follows:


As can be seen in this image above, my changes in Solder / Paste Mask have not been exported together with P-CAD ASCII. In my change, I left a spacing of 7.5 mils, in the company report says that the spacing is between 1.84 mils and the minimum rule is 3.5 mils.

Of course ... this problem can be happening due to the process that the company does to arrive in ODB ++ (converted from P-CAD ASCII from Diptrace to Altium's ODB ++). But anyway, if you have any ideas for me to solve these problems, please report.

Thanks!

PS.1: I can not post photos on the forum with the tags "[*img*][/*img*]". Generates an error message saying: "It was not possible to determine the dimensions of the image. Please verify that the URL you entered is correct."

PS.2: Sorry my English. Translate by google! ;)

Alex
Technical Support
Posts: 3897
Joined: 13 Jun 2010, 23:43

Re: Problems exporting ODB++ files and P-CAD ASCII file

#2 Post by Alex » 06 Mar 2018, 03:19

When you export ODB++ file from PCB Layout, you can change export mode. You can choose CAM software and ODB++ version. If the company can't open ODB++ files you exported please try different CAM and(or) ODB++ version.

PCAD ASCII export doesn't take care of custom mask/paste settings. We will investigate the issue.

eosrisko
Posts: 10
Joined: 04 May 2016, 10:16

Re: Problems exporting ODB++ files and P-CAD ASCII file

#3 Post by eosrisko » 06 Mar 2018, 07:19

Alex wrote: 06 Mar 2018, 03:19 When you export ODB++ file from PCB Layout, you can change export mode. You can choose CAM software and ODB++ version. If the company can't open ODB++ files you exported please try different CAM and(or) ODB++ version.

PCAD ASCII export doesn't take care of custom mask/paste settings. We will investigate the issue.
Hello Alex,

I have already tried all the options as it is in the image of my folder structure:

<a href=""></a>

I have already exported using the option "As Compressed File" enabled. I tried everything I could in the Export ODB++ window.
Nothing worked!
I do not have the company software to make my attempts. All I know is the employee's report about not being able to open the files.

About the PCAD ASCII... That's what I thought!

I'm stuck with it. I can not get a complete review of my project. Is there any solution or alternative to this?

Alex
Technical Support
Posts: 3897
Joined: 13 Jun 2010, 23:43

Re: Problems exporting ODB++ files and P-CAD ASCII file

#4 Post by Alex » 07 Mar 2018, 03:23

What version of DipTrace do you use now? Is it the latest build 3.2.0.1? If not, could you upgrade to the latest version.
Can you ask the company what CAM software do they use? This information may help us to find what's wrong in ODB++ export.
Please send your board to support at diptrace dot com.

eosrisko
Posts: 10
Joined: 04 May 2016, 10:16

Re: Problems exporting ODB++ files and P-CAD ASCII file

#5 Post by eosrisko » 07 Mar 2018, 13:13

Hello Alex,

I always work with the latest Diptrace version, in this case I use build 3.2.0.1.
About company software, they just reported.

Valor MSS Process Preparation - Versão 11.2.1.51: use for process documentation
<a href=""></a>

Trilogy, Version 9.0 Update 7: use for DFA/DFM analysis
<a href=""></a>

Alex
Technical Support
Posts: 3897
Joined: 13 Jun 2010, 23:43

Re: Problems exporting ODB++ files and P-CAD ASCII file

#6 Post by Alex » 09 Mar 2018, 03:26

DipTrace can export the latest ODB++ format 8.1 and previous 7.0. If the company uses outdated versions of Mentor Graphics tools, they may not support the latest version of ODB++ format. Do you know the version of ODB++ format supported by their tools?

eeng
Posts: 4
Joined: 03 Jul 2018, 00:16

Re: Problems exporting ODB++ files and P-CAD ASCII file

#7 Post by eeng » 03 Jul 2018, 01:37

Alex wrote: 09 Mar 2018, 03:26 DipTrace can export the latest ODB++ format 8.1 and previous 7.0. If the company uses outdated versions of Mentor Graphics tools, they may not support the latest version of ODB++ format. Do you know the version of ODB++ format supported by their tools?
Hello.

I am using DipTrace version 3.2.0.1 (Freeware) to evaluate the software.
It looks great!

I too had a problem with ODB++ export, so I asked support to our production. They found an issue with the exporter.
The UNIT directive is wrong, when you work with inches.

Code: Select all

#
#Units
#
U IN
It should be

Code: Select all

U INCH
to be compliant with the ODB++ specifications.

This directive is present at least in the profile file and in all features.Z files (layers).
I assume that other guys here work with mm and they haven't experienced this problem.
We have not tried with MM, though. I can not state if this workaround works.
Of course it could be a temporary solution, but it should work in both cases (MM or INCH) to ensure always correct output.

Could you please check?

Thank you.

eeng
Posts: 4
Joined: 03 Jul 2018, 00:16

Re: Problems exporting ODB++ files and P-CAD ASCII file

#8 Post by eeng » 03 Jul 2018, 20:09

According to my readings, there is also a difference between ODB++ 7.0 and 8.1, which are supported by Dip Trace 3.2.0.1

https://www.odb-sa.com/wp-content/uploa ... ion_v7.pdf
https://www.odb-sa.com/wp-content/uploa ... user-2.pdf

According to ODB++ specification v7.0:
U<INCH|MM>
Example:
#
#Units
#
U MM


According to ODB++ specification v8.1:
The units directive UNITS=MM|INCH can be added at the beginning of any file that contains measurable entities.

Alex
Technical Support
Posts: 3897
Joined: 13 Jun 2010, 23:43

Re: Problems exporting ODB++ files and P-CAD ASCII file

#9 Post by Alex » 04 Jul 2018, 02:30

Thank you for the report about units, we will check it. But it seems the issue is not critical. Incorrect string with IN instead INCH should be ignored, default units should be used and default units are INCH.

eeng
Posts: 4
Joined: 03 Jul 2018, 00:16

Re: Problems exporting ODB++ files and P-CAD ASCII file

#10 Post by eeng » 04 Jul 2018, 03:24

Alex wrote: 04 Jul 2018, 02:30 Thank you for the report about units, we will check it. But it seems the issue is not critical. Incorrect string with IN instead INCH should be ignored, default units should be used and default units are INCH.
I see you point. On the other hand, there are machines that work according to well defined specifications and, as it is now, they can not load the ODB++ files due to this problem with the unit.
Also, it is not efficient to correct all the files manually.
For me, it is not critical now because I've just started with Dip Trace and I don't have to arrange a production urgently. But if I suggest Dip Trace for our company, I have to ensure that the export function works without problems.

Thank you.

Post Reply