I have a question about the SIGNAL_MODEL parameter, Following the instruction in this forum I have been able to set and export the propety into PCB but when I looking at the model selection windows near the component the name of the model is present but near it is reported MODEL NOT FOUND
I will appriciate any help
In addition to assigning the model, which you did with the SIGNAL_MODEL property, you must also add the model/DML file as a reference library.To do this you have two options. The first is an environment variable named "SIGNAL_DEVLIBS" which gets set in your env file and causes Allegro to automatically included specified DML files as reference libraries. You can read up on usage in the on-line documentation.The second option is to interactively add the DML as a reference libaray. To do this open the board in Allegro PCB SI, and select the menu item "Analyze->SI/EMI sim->Library". This will open the SI library browser. In the browser select the "Add Existing Library->Local Library" button located below the upper pane labeled "Device Library Files". This will open a directory browser in which you can point to the DML file that includeds the model(s) you assigned.
I have assigned the property signal_model in capture, setting to true also the signal_model in netlist but in PCB SI I have the same report as you MODEL NOT FOUND. I have modified the variable "SIGNAL DEVLIBS" in my env file and afterall the problem continues, as djs says you can attach it directly in Allegro PCB SI following his/her instructions but in my PCB SI version (210 performance option L) doesn´t appear the menu button "Analyze" and using "tools->setup advisor->SI model Assignment" I don't see my models and there´s no Browse button. Does anybody know how could I solve this??Thank's in advanceRegards.
Try putting the .dml files in the same location as the .brd and see if that works...let us know.
Placed .dml in my working directory and set the library to point to this file. It works for me.
Hi,In release 16 or 16.01 you will have the Analyze menu in all tiers of the PCB Editor, if you're using an earlier version this menu is not available.