What gives! How do i name components of a part and have it carry through to drawing space and cut list's.
say a 8.5x11 to send to the chop-saw without any drawings just a list of lengths and tube sizes with matching part numbers. Solidworks has failed at making this a simple task.
Hi Reno
Go to the cut list in your part feature tree, right click on the list and go update to make sure the list is fully updated, now open the cut list to show all your parts, right click on a part in the cut list and select properties from the drop down menu, you will now have a list of properties for that weldment showing, add a new property with whatever information you require. I always add whatever properties I need for a weldment this way.
Paul
cut list still doesn't work, so I found another work around that has more problems. Under weldment cut list items you can select
what # to start off from, unfortunately if i bring in a different view and select a different configuration the balloons "item numbers" are all 1's
So... I went a different rout and instead of setting up different configurations to only show the weldments necessary in that part, I do a projected view of the same part/ model view and and balloons only to get all 1's again instead of 15-27 on the cut sheet.
I noticed that if i select two configurations in the model i get the the correct item numbers <as welded> <as machined> unfortunately i cant figure out how to configure the rest of the configurations the same to get the correct results.
Also i'm using the "hide" item not "suppress". Suppressing will remove the trim/ extend and render the cut list useless.
Hi Reno
Please see attached pdf file, hope this helps
Paul
Paul,
As my father used to say, "Great minds think alike" . I just this morning created a new cut list property called "Body Name". You probably already know this, but in addition to calling that property out in a balloon you can do the same with a note. I prefer to use notes over balloons because I can add another line of text or another property if I want.
Glenn
Hi Glen
I forgot about being able to use the property in a note, I normally just insert a cut list and balloon from it, but from reading the prevous posts I taught that reno wanted to use balloons, but I agree with you that using a note would be better.
Thanks
Paul
Thanks again for trying to help
Ok so your red,green,yellow does work correctly but you have to create "NAME" first before creating the weldment cut list and tagging the weldments. Then the balloons work correctly.
1. Change the configuration state of a part to as many different views you want, use HIDE to the weldments in the part you don't want to see, do this in each configuration.
two days of stress and now breathe....
Question
So when i click on auto balloon it will already be set up correctly.
Another issue I'm running into, after hiding unwanted weldment cut list items if i click rebuild they will be visible in the >cutlist< again??
Hi Reno
Hope this will help
Paul
Reno,
Here is how I do mine. I name my cut list parts by expanding "Cut list", then single-clicking on the SW-assigned name to highlight it, then a second click or the F2 key. That allows me to type in the name I want (same procedure as for naming bodies, mates, patterns, etc.). I've done that for one of the bodies in the part I threw together, see below.
You can then call out this property in a column in the cut list on your drawing. See below. Unfortunately, I don't know of any way to link it to a note. I can't find it in a drop-down. Someone may know the syntax for calling it out, but I'm afraid I don't. Anyway, hopefully this will help.