Can someone please point a semi green user to where to info on properly setting up cut lists? We have SW2015 Professional.
I am trying to set up drawings so that either the BOM or Cut list will give a total of qty of inches of, say, 2" sq. tubing or 1" dia steel or U-Channel is contained in the assembly, which consists or primarily weldments and hardware parts.
Any help will be appreciated, greatly. Thanks!
Hello,
Following along Mr. Schroeder's post, you can add the TOTAL LENGTH column to your cut list table.
(RC the table heading, insert a column and select cut list property & TOTAL LENGTH for its contents.)
On the plus side, it automatically sums each weldment profile.
On the down side, each profile's total tally is listed for each instance of that profile, so totals are duplicated, necessitating carefully review to avoid errors.
Cut lists are rather limited programmatically speaking, so redundant tallies (for me at least) can't readily eliminated.
However, you put on your drawing a cut list (for detail) and a custom BOM (for length summary).
1) Add a BOM
2) Select Indented and no numbering (number actually doesn't matter, it will be hidden)
3) Uncheck "detailed cut list"
4) Add a custom property column and select TOTAL LENGTH
5) Hide every column except DESCRIPTION and TOTAL LENGTH
6) Hide row 1 to remove the top part
Cheers,
Kevin.
Thanks, Glenn & Kevin. It seems like I have another problem, maybe. Sorry, I couldn't seem to send a DRW or a .Zip file. Any ideas about the symbols in the Total Length column?
T. Kc wrote:
Thanks, Glenn & Kevin. It seems like I have another problem, maybe. Sorry, I couldn't seem to send a DRW or a .Zip file. Any ideas about the symbols in the Total Length column?
That started with SolidWorks 2015. If there are quotations in a custom property of the .sldlfp file (the Library Feature Part file you used for the profile for the Structural Member function), which it looks like you have, it will cause that error. Edit your .sldlfp file, removing the quotation marks (you can replace them with two apostrophe's, which looks the same). Then edit the Structural Member function, re-selecting the correct profile sketch. That should fix the problem.
And for the future if you'll click on the text "Use advanced editor" at top right of the Reply box (I know it doesn't look like a link, but it is), you'll get a link at lower right to attach files. That information, along with a great deal of other stuff that can be helpful for new forum members, can be found here if you'd like to take a look.
Hello,
That's the code driving things and when SW can't solve the code, it quotes it as text.
As to why SW can't resolve this, I don't know.
The TOTAL LENGTH text is the same as the SYMBOL column text.
What does the SYMBOL column refer to? Where did it come from?
First, add the TOTAL LENGTH custom property column to your BOM to see if it resolves to a value there.
Perhaps it's not working because there's only one body. Perhaps not.
So, next try to add another body to this part and see if the total length resolves to a value.
Also, since you can't upload a file, please describe the steps you took to get where you are.
Cheers,
Kevin
I don't know if it is still current, but I had the same problem. Try to remove the "quotes".
Sq. Tube. Galv. 2"x 2" (14ga) => Sq. Tube. Galv. 2in x 2in (14ga)
Ciao,
Ariën
Welcome to the forum. There is a cut list property "TOTAL LENGTH". It sounds like that will do what you need. You can reference it with a note...
...or in a cut list column.