Summary and sharing of PCB files imported into BRD in AD software,,,,

qwqwqw2088

Summary and sharing of PCB files imported into BRD in AD software,,,, [Copy link]

 

Altium Designer software, tentatively called AD software, has been upgraded many times since it merged with PROTEL99. There are various versions. When importing Allegro circuit board PCB files (suffix brd), many problems will arise, and there are many cases where the import fails. Sometimes even if the import is successful, there are many problems, such as the design rules are not imported. AD's PCB file (.PcbDoc) contains design rules, and Allegro files (.brd) should also contain design rules, which are incompatible after import. The package library is generated from the imported PCB file. The components in the library are messy, not only containing the basic elements of the components such as Pad and Outline, but also many unnecessary things, even wiring and via. It still needs to be sorted out. And different versions of the two software will have format incompatibility. Now I will share some successful import experience and tips to provide you with some reference. It may not be suitable for the import of all versions of files, but just some experience in importing in AD15 version. First, let's start with some FAQs. Let's answer some common questions first: Q: If you have installed Altium Designer, can you import Allegro's PCB files? A: Not necessarily. If it is a PCB in *.brd format, you must install the Cadence suite on the same computer; if it is a *.alg format that has been converted, you can import it directly. Q: Can I import brd files without Allegro installed? A: No. However, you can use extracta to convert it to alg format on a computer with Cadence installed, and then import it. Q: Which versions of Allegro does the importer support? A: Supports 15.2 and 16.x. The latest AD19 currently supports some 17.2 files. Q: How accurate is the conversion? A: About 90%. There are generally no problems with basic components, routing, and networks, but it will be less accurate for Polygon, special-shaped pads, and some special objects. Remember, any format conversion will inevitably require a lot of follow-up work. Second, before the formal conversion, you need to confirm whether the preparations are ready. Installation of Importer When installing the software, make sure the Importer/Exporter option is selected (it is checked by default). After correct installation, you can see the supported import and export tools in Extension & Updates. For example, the AD15 plug-in is as follows

qwqwqw2088

Third, the process of installing the Cadence suite import is actually divided into two steps: Use Cadence's extracta.exe tool to convert the binary brd file into an ASCII alg file. The AD software parses the alg file and generates the final pcbdoc file. Since extracta.exe is a tool provided by Cadence, the Cadence suite must be installed. Don't try to copy only one extracta.exe, which is completely invalid, because extracta will also call other dlls, so the easiest way is to directly install a Cadence suite. The Cadence suite that needs to be installed is not necessarily the professional version of Allegro, it can also be a completely free version. There are several ways to install the free version, which can generally be found on Baidu. After the installation is complete, there is no need to connect any license. There is only one purpose, installing Cadence is to call the conversion function of extracta. Set environment variables To ensure that Altium can find the extracta tool correctly, you need to set two environment variables. Right-click "My Computer", find "Advanced System Settings" in Properties, and click "Environment Variables":

Add two new variables in the system variables (the variable name is before the equal sign, and the value of the variable is after the equal sign): TELENV = C:\Cadence\SPB_17.2\share\pcb\text\env PATH = C:\Cadence\SPB_17.2\tools\bin The value of Path is the folder path where extracta.exe is located.

If Altium Designer and Cadence are not installed on the same computer, it is impossible to convert the brd file directly.

There is a workaround. Find a machine that has Cadence installed, convert the brd file to alg format, and then import it in AD. The specific steps are as follows: Under the System menu in the AD installation directory, find the following two files: Allegro2Altium.bat AllegroExportViews.txt Copy these two files to the computer where Allegro is installed, run cmd in the same folder as the brd file to be converted, and cd to the folder where the brd file is located in the DOS window. Run Allegro2Altium xxx.brd (xxx is the brd file name). The system will automatically run and generate an alg file with the same name. If an error occurs during the conversion process, it is most likely due to the Allegro version. For example, extracta 17.2 cannot convert brd files from 15.2, and vice versa. Is there any solution? The only way is to install several different versions of Allegro

qwqwqw2088

4. Start the conversion After everything is ready, you can start the conversion. The conversion process is relatively simple with the help of a wizard. Click File ----Import Wizard, run the wizard

Select Allegro Design Files as file type:

Add the PCB file to be converted (brd or alg format)

nextNext, the importer will analyze the file. If an error similar to the one shown below appears during this process, there are only two possibilities: - The Allegro version is incompatible - The environment variable is not set correctly.

If everything is normal, the interface of setting report will pop up. You can view the detailed information of conversion in log:

Next, we need to deal with some features that cannot be recognized during the conversion process, such as the connection method between pad and Polygon and Plane, whether to automatically generate polygon cutout, etc. Everything is OK, and it's done!

V. Cleanup The conversion is complete but it does not mean everything is fine. There is still a lot of cleanup work to be done. The following is a recommended checklist: Physical check: Check the board shape and the shape of the cut slots. As mentioned in the previous article, special-shaped pads may cause errors during the conversion process. Are the device packages and sizes completely consistent? Electrical check: Mainly check whether the network is correct? Rule check: Are all rules imported correctly? DRC check Check the settings of Polygon for hot pads and whether they are directly connected Check the settings of the power plane for solder mask and solder assist Via Tenting rules Test point distribution Power check: Power network Power plane Copper Polygon Document check: Layer string Graphic identification, etc. PCB report Whether the number of devices/networks is consistent with the original image Whether all networks are connected VI. Summary After mastering the key nodes, it is not so troublesome to convert Allegro's PCB to Altium, and the results are completely acceptable. The question is, since Altium can import Allegro's PCB, can Allegro import Altium's PCB? The answer is yes! After version 16.6, Cadence added an "Altium to Allegro PCB Translator" for Allegro. As long as the AD file is saved in ASCII format, it can be converted to Allegro's brd file using this converter. The only problem is: Altium's ASCII file is a version from many years ago, and it seems that it has never been updated (as can be seen from the prompt when saving). This means that the elements and functions supported in the new version of AD are not reflected in the ASCII file. If there is a deviation in the recording of this information, it may cause deviations in the converted PCB file. Of course, there should be no problem with basic components, networks and wire connections (the editor has not verified it personally, lacking MONEY). Another very annoying thing is that all modules of Cadence are charged, and this one is no exception! The beggar version of the suite does not even have this converter! Although Cadence is stronger than Altium in many professional fields, can it learn from Altium in the module charging link: one license, all modules! Taking a step back, can some commonly used and easy-to-use modules be made available for free?

倾心思梦

Thanks for sharing!

懒猫爱飞

Very good, thank you for sharing!

一壶漂泊1314

Hello, I would like to ask how to convert the binary brd file into an ASCII alg file using the Cadence extracta.exe tool?

qwqwqw2088

一壶漂波1314 发表于2019-4-25 15:31 Hello, I would like to ask you how to "convert the binary brd file into an ASCII alg file using the Cadence extracta.exe tool."

I really don't know how to convert this. Waiting for other friends to share

电子地瓜

Thank you so much, I searched for a day. I finally solved the problem of not finding candence

generalcircuits

I got this from another post. Thanks for clearing up my confusion. Very good information.

afeionline

Thanks for sharing