Hi,
Is there a way to change the property name for all my weldment profile ? I would like to change from Description to DESCRIPTION, so when I create a cut table all my table heading is in capital.
Hi,
Is there a way to change the property name for all my weldment profile ? I would like to change from Description to DESCRIPTION, so when I create a cut table all my table heading is in capital.
I think the only place this can be done is in the Weldment Profile Template.
you can also add additional custom Properties.
Hello Emilio,
I believe the easiest option would be to create a new weldment cutlist template.
Open a drawing and insert a weldment cutlist table. Format it as you would like it to appear and then save it as table template.
After you have created the template, click into the solidworks options -> file locations -> weldment cutlist templates and add the location where you have saved the weldment cutlist table template.
The next time you insert a cutlist, it may automatically use the default one, before clicking the green check mark select the browse option and select the template that you created.
You can also use the same process for BOM table templates, the only difference is that you add the location to 'BOM templates' from the drop down in 'file locations'.
Hope this helps,
Stavros
Hello Emilio,
You can use #TASK to do the job. Please find a short demo video in the attachment. You need to use 'Custom Properties Manager' task which is a part of the #TASK Standard plan (free).
Please backup your files before runing batch rename task.
Thanks,
Artem
Try this.
Go to Tools, Options, select File Locations then Custom Property Files
Browse out to the folder listed and open properties.txt and either change the existing Description to upper case or add DESCRIPTION. This will only update new models. It would be easier as Andreas and Stavros suggested and update you template.
Very nice to have so many people trying to help ! Thanks guys for your time, really helped a lot.
I have another question, maybe you guys know a quick and efficient way to update a hole categories of weldment profiles. Is there a easy way to change the description of all square tube ? like adding (portuguese) TUBO QUADRADO before the standard description ?
Hello Emilio,
the way Solidworks has them setup, you would have to open each profile individually and type them in individually.
If you copy one of the profiles, preferably the smallest, you can then use a design table to have all of the profiles (for SHS) in one file. In that case you can control the descriptions by linking the cells in the description column to a combination of cells to get the desired description.
Kind regards,
Stavros
Thanks Stavros !
How can I change the profile size after I used a profile with a design table ?
Hello Emilio,
They are setup as configurations, to view the different profiles within the file just cycle through the configurations.
To add it to your profiles, you could create a custom profile folder and add it to 'weldment profiles' section in options>file locations.
When you insert a beam, it should show up as all the other profiles do. If you have setup a custom profile folder you will just have to select your custom profiles from the drop down, then profile then size. The index is optional, I prefer it as it organizes them by size in the selection drop down when you want to insert a beam.
Kind regards,
Stavros
I think havent been clear with my question, I used the profile that you send to make a test but after using it in a new weldment part I couldnt find the option to change the configuration as it is in your design table.
Bellow you can see that just the first configuration from your design table is set, I couldnt find the way to change to a bigger profile.
Hello Emilio,
You can select the size before you place it. If you have already placed the beam, as it appears in your screenshot, you will need to right click 'edit feature' and select a different size from the drop down
Hello Emilio,
I notice that when I insert beams on my machine, it calls it "Square Hollow Section - configured 'Description' ". Yours does not seem to indicate that it is configured, try testing the file that I attached and see if it works.
Kind regards,
Stavros
Ohh ! I have saved the profile in the square tube folder, now I understood I have to place it in a folder before.
It worked ! Thank you again Stavros,
Best Regards
Emilio Janssen
Hello Emilio,
I couldn't remember if that was a requirement or not, for our profiles I had setup a custom folder location, that must have been why I did.
Glad I could help.
Kind regards,
Stavros
Hello Emilio,
I believe the easiest option would be to create a new weldment cutlist template.
Open a drawing and insert a weldment cutlist table. Format it as you would like it to appear and then save it as table template.
After you have created the template, click into the solidworks options -> file locations -> weldment cutlist templates and add the location where you have saved the weldment cutlist table template.
The next time you insert a cutlist, it may automatically use the default one, before clicking the green check mark select the browse option and select the template that you created.
You can also use the same process for BOM table templates, the only difference is that you add the location to 'BOM templates' from the drop down in 'file locations'.
Hope this helps,
Stavros