You can assign custom property fields to balloons. Just remove the circle style.
One possible solution:
1. In the new sheet, create a phanthom drawing view of the weldment.
2. Attach a note to the body in question (with a leader)
3. In the note type $PRPWLD: "name of property"
4. Move the drawing view outside of the sheet space
5. Hide the leader and move the note wherever you need.
Note: most likely this workflow can be simplified a lot.
To expand on what Alin has said:
We do similar type annotations and it should be straight forward (although cutlist property manipulation can be flaky at times).
In our multi-body weldment part, we have added custom properties in the cutlist properties for each body.
In the drawing, we have a view of the complete weldment multi-body part along with a cutlist. You aren't required to have the overall view. But if you don't have the cutlist in your drawing (it does not have to be on the same page as the individual body views) then this technique will show the custom property of the overall part file, not the body specific property - at least that is the behavior I have observed.
Create a new view. Select the weldment part and click the next arrow in the model view property manager. Under the Referenced Configuration section click the Select Bodies button and pick the weldment body you want in the view from the model.
Once the view is created attach a note to the body. The note needs to attach to the body with a leader - you can hide it later. Just placing the note in the view will not associated it with the body specific properties. In the note type $PRPWLD:"name of cutlist property". The PRPWLD must be in all caps.
As soon as you complete the closing quotation mark the note should show the cutlist property value if all is well in the universe. You can now select the note again to launch the note's property manager and change the leader type to hidden if you don't want it.
You can copy and paste this note to other individual body views. If you have hidden the leader, you will need to temporarily re-show it, attach it to the body, and hide it again.
If you find a situation where you are sure things are correct and the note either will not show or will not update or some other odd behavior, restart the SW session. We are still using SW2011 so perhaps this occasional behavior has stabilized in the newer released.
Hope this helps.
Thank you. I had already brought in the drawing view using the Select Bodies function (one of my favorite SW2010 improvements), so I picked your directions up from that point and it worked well. I saved the note to my Design Library and it worked fine when I attached it to another drawing view.
And I appreciate the very detailed instructions using small words. It's been a long week.
Your response was good also, and I wish I could give credit to both of you for the right answer. I gave it to Daen because his directions fit my workflow a little bit better.
No worries, Glen. I liked Daen's post myself.
This is (so far) the best approach I have seen to detailing weldments, but there is still room for improvements to better adapt the processing of detailing weldments to our specific company needs.
We use a lot of aluminum extrusion, which is designed as a weldments in SW.
When comes time for manufacturing, we need a different drawing, and a different part number for each structural member.
There are a few ways to do this, and I've actually completed a project using each approach. However, I still find myself looking for a better way to do this.
1) I tried the good old 'insert into part' method. This essentially creates a new part of the structural member.
When designing a large weldment, RMB-ing each structural member and inserting into part is actually quite time consuming. Also, the individual structural member custom properties that were set in the main weldment file are not passed to the new, individual part files. So all custom properties have to be entered in each individual file. Another con is the massive number of separate part files that this method creates.
2) I tried creating an assembly from the weldment. This technique sounded quite promising, until I realized that the advantages of the cultist (ie. having SW auto-detect identical structural members) is lost. When converting a weldment to an assembly, every structural member (even if there are identical) is inserted into the assembly as a different part. Not so good.
3) the last project I did, decided to make a single drawing for the weldment.
I put the overall weldment on sheet1, and added relative views of each body on separate sheets. This way I ended up with 1 structural member per sheet. So far so good.
From the weldment file, I right clicked the cultist, properties, and added the part numbers for each individual structural members as custom properties. Finally, I used the technique described in this discussion to show the individual structural member part number property on each sheet.
Is there a better way of doing things?
is there a way to have the individual body part number show in a sheet format, if the only thing on that sheet is the body in question?
I'm still looking for the best way to model and detail complex weldments quickly, while meeting the manufacturing requirement of having one drawing, one part number per structural member.