Every time I place a new flatpattern view into a drawing from a new configuration it creates a derived configuration with the suffix "SM-Flatpattern" and I would like to change this. Is it possible?
I do not know if it is possible to change the default prefix. But you could give it a try to use the IConfigurationManager and/or IConfiguration interface. However, you need then a way to execute the code you have written. Either by events or manually by pressing a button.
I am concerned that using either of these methods would only create an extra configuration instead of modifying the existing one that is automatically created on the drawing sheet. I am trying to avoid having a build up of unwanted configurations. Is there not a file I can access to change what it names the flatpattern configuration?
No that I'm aware off. Looking deeper into the forum I found that this has been discussed before... but they kind of just accepted the naming,
Perhaps Deepak Gupta have some insights in this.
You would think that if you can access the Bend notes text file, you should be able to access the file that creates the automatic configs. This is disappointing
Well... another idea is that you search thru the windows register and the text and xml files in the Solidworks folders.
Or contact you Solidworks support (VAR). They should be able to give the final answer if it is possible or not.
Brandon, I would like to know as what issue you've with that naming convention.
When I create drawings for specific parts, I like to show a detail of the part number I place on the part. Typically the flatpattern is the best option for that. Since I have so many configurations, I link the text in the part number to the configuration name. I would like the part number to reference the part number that does not have SM-Flatpattern in it.
One thing you could do is if you are using configurations then I would link the note to a configuration specific custom property like "PartNo" instead of the configuration name. We use configurations very heavily, and all of our configurations are named after the part number. So in our sheet metal parts, instead of having to worry about the "SM-FLAT-PATTERN" attached to the end of the configuration's name, we use the custom property of that configuration. If your files are not set up this way and you would like to use a macro instead, delete the linked note out of your sheet format and run this macro on a sheet metal drawing.
We use Design Tables for everything so I guess I could place a $PRP in the design table and link the part number to that custom property. Thank you everyone for the help, I will also take a look at your macro Adam and see if it will be beneficial for our operation.
A simple solution, make the derived flat configuration manually and name it whatever you want. Don't let the drawing make it for you.
You can even make a template for sheet metal parts with the derived configuration already a part of it.
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