Protel package library conversion to allegro package library
Using Protel for PCB design for a long time, we will always accumulate a large number of Protel package libraries that have been proven in practice. When the design platform is converted, how to retain this package library is always a headache. Here, we will use Orcad Layout and Layout2allegro to complete this work. The steps are as follows:
a) Place the PCB package in Protel (you can place all the packages that need to be converted at once) on an empty PCB, and export this PCB file in the format of Protel PCB 2.8 ASCII;
b) Use Orcad Layout to import this Protel PCB 2.8 ASCII file and save it (.max);
c) Use Layout2allegro to convert the generated Layout .max file to Allegro’s .brd file;
d) Open the newly generated .brd file in Allegro, select Tools>Padstack>Modify Design Padstack in the top menu, and you will see the name and number of the current pad in the Options tab (starting from 24.pad and increasing one by one). Select one by one, click “Edit”, and activate Padstack Designer to edit the selected .pad.
e) For surface mount pads, first check the Layers tab to check if the pad already exists in the library or can be replaced with a .pad that already exists in the library (a difference of less than 1/10 is acceptable). If not, then:
① In the Parameters tab, change the Type option from “Blind/Buried” to “Single Item”;
② Unit section: Select Mils for Units and enter 0 for Decimal places, indicating that the unit used is mil, with no decimals after the decimal point, i.e. an integer;
③ In the Layers tab, delete all layers between Top and Bottom except the Default Internal layer; adjust the Regular Pad, Thermal Relief (6Mil larger than Regular Pad), and Anti Pad (6Mil larger than Regular Pad) on the top layer; Regular Pad on the Soldermask_Top layer (6Mil larger than Regular Pad on the Top layer); Regular Pad on the Pastemask_Top layer (same as Regular Pad on the Top layer); Pad), confirm that the data of other unused layers is “Null”; (For surface mount pads, only Top, Soldermask_Top and Pastermask_Top need to be set)
④ Save the newly created pad according to the naming format of the .pad file, and save it in the path recognized by allegro set in the environment variable;
⑤ Select Tools> Padstack> Replace in the top menu, click the Pad just modified, and the name of the Pad before the change will appear in the Old option of the Options tab; then click the button behind the New option, select the newly created Pad, and finally click the Replace button below to complete the update of this Pad.
For the pad of the via, first check the Layers tab to check whether the pad already exists in the library or can be replaced with a .pad that already exists in the library (the difference is within 1/10, which can be considered). If not, then:
① Confirm that the Type option in the Parameters tab is “Through” (or define it as “Blind/Buried” depending on the design needs);
② Unit part: Select Mils for Units, and enter 0 for Decimal places, indicating that the unit used is mil, with no decimals after the decimal point, that is, an integer;
③ In the Layers tab, delete all layers between Top and Bottom except the Default Internal layer; adjust the Regular Pad, Thermal Relief (10Mil larger than Regular Pad), and Anti Pad (10Mil larger than Regular Pad) on the top layer; copy the Top layer information and Copy to all, then you can set the three layers of Top, Default Internal, and Bottom; adjust the Regular Pad of the Soldermask_Top layer (10Mil larger than the Regular Pad of the Top layer) Pad is 6Mil larger) and copied to Soldermask_Bottom layer; (For via pad, Pastermask_Top layer does not need to be set)
④ Save the newly created pad according to the naming format of .pad file, and save it in the path recognized by allegro set in the environment variable;
⑤ Select Tools> Padstack> Replace in the top menu, click the pad just modified, and the name of the pad before the change will appear in the Old option of the Options tab; then click the button behind the New option, select the newly created Pad, and finally click the Replace button below to complete the update of this Pad.
f) Replace all pads according to the method of item (e) above;
Note: Since allegro generates a library file each time, the name of its .pad file is increased from 24.pad until all pads are output. If you perform two or more library file generation operations, the .pad file generated by the latter operation (starting from 24.pad) will overwrite the previous .pad file, resulting in the pad being replaced when calling the previously generated library file .dra. Therefore, after exporting, you need to re-create the .pad file from the .dra file and replace the pad in the .dra with the newly generated .pad file to ensure the correct use of the library!
g) Next, we use Allegro’s Export->libraries function to output the package library .dra, .psm, etc., and the pad library .pad, and then after h) operation, add ref, etc. to complete the conversion of Protel package library to Allegro;
h) “Designator” in Protel is converted to Silkscreen_Top and Display_Top of Ref Des under Components in Allegro; “Comment” is converted to Silkscreen_Top and Display_Top of Part Geometry under Geometry. At this time, delete the two “Designator” and two “Comment”, add “REF” to the Silkscreen_Top layer of Ref Des, and add “DEV” to the Silkscreen_Top layer of Device Type;
i) File>Save as generates a .dra file according to the component naming rules and saves it to the allegro component library directory;
j) File>Create Symbol generates a .psm file and saves it to the same directory as .dra.
The process of importing Protel components into Allegro is now complete, and the newly generated library file can be called in allegro. In Allegro, .dra files are organized through .pad files, and .psm and other files are generated through .dra files before components can be called. Therefore, when using components, pay attention to the corresponding relationship between each part to avoid mismatching such as incorrect calling of .pad.
