I need to make a custom Properties Template wich should look like in the picture. Is there a way to enter manually the Drawing Number anb Revision and the Part Number captures this infos and populate automatically?
very powerful note tool for building title blocks.
the only thing that you need to add to your property tab builder is the stuff that would need to be edited, modified or changed.
i used to be able to put all the info for the title block in my parts and assemblies. No mater what title block i would drop them into it would be filled out automatically, Every now and then it would need some custom spacing for 2 line descriptions. I even found the special SolidWorks chatterer that would do that. Change a logo on a title block, change the company name, address, or other standard notes, tolerances, update the template save out a sheet and then every time you open an old drawing, reload the sheet or replace it with the new one.
If you don't have the Part Number in the tab builder you can create your part number in the custom properties tab by using $PRP:"Drawing Number" $PRP:"Revision". What is in the quotes should be the Property Name you use to define those items.
So if your property name for Drawing Number was DRAWNO and the property name for Revision was REV it would look something like this in the custom properties $PRP:"DRAWNO" REV $PRP:"REV". If your drawing number was Example-000 and the Rev was 0 it would come out like "Example-000 REV 0"
PS. I only say to not have the Par Number in the Tab builder because I've been running into issues with having info in the property tab builder not evaluate in the custom property tab.
Thank you. I know that. But if you don't have the Part Number in Custom Properties, it won't appear in BOM under the column Part Number.
Is your Part Number different then File Name??
Here I have them the same then it's easy to call $PRP:"SW-File Name"
Yes, the file name has the Part Number with a brief description. I don't need that desciption in my Part Number.
Then you'll need to input it manually, good chance for typo's ...
If it's the only way, I'll live with that.
The "Only" way that I see is to keep any description out of the File Name - but that's just my 2 cents - Then it's all automatic, re-typing = potential disaster later...
It's not my call, it's the company policy.
You can put the part number part of the filename in a custom property if you have a standard naming convention.
We have a macro that we modified from one of Deepak Gupta's. I started with the ones from this discussion:
File name into a drawings sheet... with slight changes.
File name into custom property with a slight edit...
This one might also be helpful:
Extracting filename to custom properties
We updated the property names to match ours. I added an if statement to remove anything after the first _ since we name our files as PN_Description.
too much for too little.
thank you anyway.
If you put the $PRP:"DRAWNO" REV $PRP:"REV" in the "Value/Text Expression" in the custom properties with the Property name of "PARTNUMBER" then you can pull into the BOM. I would add the $PRP:"DRAWNO" REV $PRP:"REV" to my part template under custom properties. It would be in the custom properties. Then when you add the DRAWNO and REV into the custom tab builder the PARTNUMBER would be created on rebuild.
Added "PARTNUMBER" to our template. Description and heat treat are added in the custom tab builder.
Add info in the tab builder. Apply and Rebuild.
Part number is created. Pull that into your BOM.
As a side note if you can't add the $PRP to the template you can create a list in your custom tab builder having the only choice being the $PRP info. The only glitch to this is that it puts it into the custom properties but does not evaluate properly. You have to go into the custom property and modify it. Any modification will make it evaluate properly. I think this is a SW bug. Oddly enough if you type it in directly it does evaluate properly.
it works well for me. job done.
Does it evaluate properly? I've done this a couple times and it enters it into the custom properties properly but you have to go in and modify it there. The last time I tried it it was in cut list items for weldments though so maybe it works for parts.
I've tried few times, it worked well.
Thank you. That is what I was looking about. So, you create a Note with the text/link that you want and, after that Copy-Paste this Note in the Tab Builder. It worked well.
HAS anyone found a way to add a formula to the property tab?
i have to take the weight of some assemblies and multiply x 1.3 and the do some rounding that i would really like to automate.
I do that in my equations. Would that work for you?
As Jim Steinmeyer said, you can create an equation with your formula, after that you create a Custom Properties linked to your equation and save your Part/Assembly Template.
I don't know if you can put this formula directly in the Tab Builder.
may be worth checking into next week
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