Linked properties in General Table

I am having trouble following your process... Are you linking the Custom properties of a part to an external Excel sheet, or is the data inside a Design table within the Part file?

The other question is are you using SW PDM or another type of PDM system?

Scott Baugh, CSWP
Mechanical Engineer
Ciholas

"If it's not broke, Don't fix it!"

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faq731-376

Treads0322,

You should be able to interrogate SolidWorks and extract the volume of your part, as a parameter. If you add the percent fibre, you can work out the volume of resin and fibre in your finished product. This does not account for wastage. Are your CAD guys going to fill in your data?

--
JHG

@SBaugh - the goal is to show the data from a custom property in the .sldprt in a general table on the drawing. Desired result is below:

Here are the properties feeding it:

The surface area is filled by a global variable which takes SW-calculated surface area of the part. All the qty values are calculated by formulas in the table.

My goal is to save the table format so that I can insert it into a new drawing, associate it with a view, and keep the custom property links. Right now those cells all come out blank; the only cells that are filled are the plain text (header / row titles and units column) and the formulas (all zero since the sq. in. property is missing). If there's no way to save that linked property in the .sldtbt, then I'll create another macro to fill that out rather than doing it by hand, it's just a step I was hoping to find a workaround for.

Yes I'm using PDM, do you see that making a difference to use of the table template?

@drawoh - as above, I'm interrogating SW for the surface area and calculating the rest from that, including a % multiplier for wastage. The challenge is getting the linked property into the table without manually filling setting the value for that cell for each drawing.

Add the table to the drawing template. Add custom props to table and parts. When add the parts to the dwg, it should read the props.

Chris, CSWP
SolidWorks
ctophers home

@ctopher Good suggestion! I like that option for new drawings; we don't currently have separate templates based on part type, but I have some similar work to do with providing more stock material information for sheet metal parts, so it may save some time to create all of these as separate templates. Unfortunately, I still have to deal with existing drawings, as we frequently copy an existing part / drawing and change the color or trim for a new project, but if I have to use a macro to fill those I'll live with it.

With PDM you might be able to add some of that data into the data card. I use an equation in my BOM to know which part number to use. It can either be our CPN number or Supplier number, by using a single check mark in the data card. "IF(`Purchased`=0;`CPN`;IF(`Purchased`=1;`Sup_PartNo`;`CPN`))".

Most of my custom properties are controlled from the data card. Then I link the BOM or areas of the drawing to the custom properties of the part or assembly that is supplied from the Data card. It might be nice to have that data linked to the card giving someone easy access to read the data there instead of looking at the drawing/table.

Scott Baugh, CSWP
Mechanical Engineer
Ciholas

"If it's not broke, Don't fix it!"

Click to expand...

faq731-376