I search the KB about this and came up empty. Does anyone know how to link a note to a weldment custom property? Is that possible?
Gents, create a note and point to the weldment part, then type the following:
$PRPWLD:"DESCRIPTION" shows the Description of the body based on the cut-list.
$PRPWLD:"LENGTH" shows the overall length of the body based on the cut-list.
You can use pretty much anything in side the quotes as long as it excists in the cut-list properties.
Let me know if it works.
Timothy, I have explored this in quite some depth, and I have not found a way to do so. So, unless someone can prove me wrong, I'm sorry but it is not possible.
There are however, alternatives...you can possibly create a macro to fetch these properties and process them as you wish...
Hmmmm... I was afraid of that. Perhaps if everyone who sees this posting goes to the 'Enhancement request' section and puts in a request, then SW will get that fuctionality built into the software soon.
I've just psted the Enhancement request' myself.
Hi John, $PRPWLD seems to do the same as $PRPSHEET...I cannot get it to work on my system...can you show some snapshots of this working?
Are you sure it's picking up properties from the weldment and not the document?
Aha! I figured it out. SW requires that you type the code into the note in ALL CAPS.
So the code has to be like this:
or else it does not work.
Learn something new every day!!
Did it work for you?
John, no...I haven't been able to figure it out...not working...
The bahaviour is the same...when linking notes in bom or/and from drawing...
I also tried deleting the model custom property to guarantee it wasn't overriding somehow...but it wasn't...
See attached image...
Have you considered using a balloon, withoug the shape? You would however need to insert a cut-list onto the sheet somewhere, and then in the balloon properties, using the custom properties and selecting which one you wanted to use?
Thanks for the suggestion. Unfortunately balloons take custom properties from the part, not the cut-list properties. Perhaps the enhancement could include cut-list properties in a ballon. I would rather see it as a note so you can add multiple lines instead of just one on the balloons.
John, I would still like to see how you managed to link to these weldment properties...if you don't mind.
Hello John, are you sure that you had inserted a cut-list table? you should definitely be able to pull properties from the weldment cut-list.
No problem inserting a cut-list in a single part weldment but I cannot inside an assembly. The only way to have cut-list items show up in an assembly is to click on detailed cut-list. Of course we can't extract that info inside the assembly - just the properties of the individual parts, not the cut-list properties.....
you're absolutely right...there must be a weldment cut-list inserted for the model you want to get properties from otherwise it will just behave as if you were trying to collect properties from the part and not the weldment.
By the way SOLIDWORKS...this is the stupidest F'n sh$T I've ever seen...if you're going to implement a system accessor like $PRPWLD...then make it work in a consistent way, why in the F$$K would I have to add a cutlist for this to have to work? I can't believe I spent 3 hours + trying to get this to work...and it was just something this simple...
What if I want to get these link within the part itself...where I can't add a cutlist?
Solidworks...you have been letting me down...day after day...
Anyway...it works now...I'm glad I figured it out!
Thanks all, for your help!!
Gotta love honesty. I agree - I could write a book about "work arounds" it seems. I think they concentrate too much effort in getting "new" stuff into each release and don't spend enough making what is there work as it should. Don't get me wrong I love SW and will continue to use it but I sure wish they listened to us "users" a bit more. For example - when you mirror a part you can check a box that says to carry over custom properties but it seems they are part properties not cut-list properties - cool if that worked....
Anyway - we can help each other in the meantime. Maybe SW 2012 will have no new features and expaned current features....LOL.
Yup, I agree with you.
One thing worth mentioning though, is that ...if this really is bothering you, and it interferes with your daily work...it's worth calling your VAR and mention it...so they can look into it and see if there is any SPR or ER already on this...and if there is, they can add your name to the list.
Complaining on this forum (like i just did...lol)...really doesn't do much...what really gets the problem solved is "signing" your name on these SPR/ER...which increases the priority for this problem. I'm just too lazy to do this...and lost drive...since there are so many little problems like this and I just don't have time to be on the phone half the time with my VAR...
I need a drink...is it 5 o'clock yet? hah
Actually, laziness is no excuse.
You can easily submit an Enhancement Request yourself directly right at list link:
In fact, I've heard that an ER submited directly by a customer counts for more than one submitted by a VAR.
So everyone.... go for it!
Tried to look at your attachment but I am still on 2010.... : )
Have a look at my attachment. Very crude weldment but shows the point. The $PRP.... takes info from the cut-list, not the part. Open up the drawing and see if it works for you. Try to copy/paste the note from mine onto your drawing and see what happens. Report back....
I am using SW2011 SP3.
I just ran into some issues and a search of the forum brought me to this thread. I wanted to capture my observations.
I have a multi-body weldment file. I created a drawing for it that showed the whole multi-body part and a weldment cut list on the first page and the subsequent pages showed each body individually. For the individual body pages I used the "select bodies" button when placing a new view of the same weldment. On each of the individual body pages I attached a note that pulled weldment data. In my case $PRPWLD:"NAME". This all worked just as you would expect.
I have eight drawings all documenting very similar weldments of rectangular tubing. This attached note process worked without issue in all of them
Now I am working on a drawing for a multi-body weldment and the attached notes show up blank. This weldment has different cross sections; channel, angle, flat plate. I can't imaging that should make a difference. As before, the first page represents the whole weldment. I created an "exploded" configuration in the part file and used the copy/move bodies feature. The second page of the drawing shows this exploded configuration and contains a weldment cut list. I can add the $PRPWLD... notes on this second page and they populate correctly. The following pages again document the individual weldment bodies using the "select bodies" functionality noted above.
These pages of individual bodies will NOT populate the $PRPWLD:"NAME" note. However, if I add a weldment cutlist to the page the note is on and perform a forced rebuild, the note will populate. Delete the cutlist from the page and force another rebuild and the note blanks...
Not quite sure the difference between this latest drawing and the others that worked correctly.
My current work-around is to place a weldment cut list off the printable area of each page.
Gotta luv it...
One additional observation:
I used the built-in End Cap capability for some tubing. Trying to place a note in the drawing for just the end cap gave the same blank result. So I added the welment cut list off the printable area of the page. The cutlist is not populated nor is the note....
Retrieving data ...