Ballooning a weldment with hidden parts
Ballooning a weldment with hidden parts
(OP)
Hi everyone,
Looking for a best practice for my current situation:
I'm designing a lot of parts with weldments and sheet metal parts all together in one part (instead of an assembly). It works perfectly fine for the modeling process, but it becomes a pain when I want to do a set of drawings on how to assemble these creations.
I can use configurations to setup the part with different pieces shown/hidden, but i found that to be inconsistent; I'd get parts re-appearing after switching configurations, sheet metal flat patterns often showing other parts shown when they should be hidden etc. At the very least I need to be able to hide my sheet metal parts to be able to call out the weldment pieces behind them.
I recently tried to use display states instead of configurations, and while it's quicker to setup and get going, when i point a balloon to a weldment part, it will "see" the hidden sheet metal part that's in front of it first, and use the item number of the sheet metal instead.
I've also started using configurations and the delete body feature instead of hiding parts. This works well but is slower than the other 2 options, and adds features that makes it annoying when i make changes to a design.
Anyone else encounter this kind of situation? how do you deal with it? My industry is pretty fast-paced, so speed is the priority, while keeping accuracy and avoiding having to hand-type any numbers in a drawing to keep it parametric,
Thanks!
Looking for a best practice for my current situation:
I'm designing a lot of parts with weldments and sheet metal parts all together in one part (instead of an assembly). It works perfectly fine for the modeling process, but it becomes a pain when I want to do a set of drawings on how to assemble these creations.
I can use configurations to setup the part with different pieces shown/hidden, but i found that to be inconsistent; I'd get parts re-appearing after switching configurations, sheet metal flat patterns often showing other parts shown when they should be hidden etc. At the very least I need to be able to hide my sheet metal parts to be able to call out the weldment pieces behind them.
I recently tried to use display states instead of configurations, and while it's quicker to setup and get going, when i point a balloon to a weldment part, it will "see" the hidden sheet metal part that's in front of it first, and use the item number of the sheet metal instead.
I've also started using configurations and the delete body feature instead of hiding parts. This works well but is slower than the other 2 options, and adds features that makes it annoying when i make changes to a design.
Anyone else encounter this kind of situation? how do you deal with it? My industry is pretty fast-paced, so speed is the priority, while keeping accuracy and avoiding having to hand-type any numbers in a drawing to keep it parametric,
Thanks!






RE: Ballooning a weldment with hidden parts
RE: Ballooning a weldment with hidden parts
Good luck
Patrick
RE: Ballooning a weldment with hidden parts
That's interesting. To me its one of the tools I like the most! Use it almost daily! And I usually create separate views of each body in the weldment. Wham bam. In fact, I like multi body parts so much I will often model single body parts that way just to make it easier for me.
RE: Ballooning a weldment with hidden parts
Hope that helps,
Scott Baugh, CSWP
FAQ731-376: Eng-Tips.com Forum PoliciesGryphon Environmental
www.2gryphon.com
www.scottjbaugh.com
RE: Ballooning a weldment with hidden parts
Do you have a drawing file with multiple sheets for each parts? The workflow we are using here requires a separate file for each part that's why I don't like having multiple parts in the same file.
Patrick
RE: Ballooning a weldment with hidden parts
Scott Baugh, CSWP
FAQ731-376: Eng-Tips.com Forum PoliciesGryphon Environmental
www.2gryphon.com
www.scottjbaugh.com
RE: Ballooning a weldment with hidden parts
What Sbaugh said. Set up your views to show selected bodies only. You can have as many sheets and as many views of as many bodies as you want. You can even identify those bodies in those views with balloons that tie back to the main cut list. We usually also show the As Welded and As Machined configurations on separate sheets.
Does your workflow actually require a separate FILE for each body? Would a separate SHEET fulfill the need?
If your system does indeed require a separate electronic file for each part I would consider a couple options:
1) When you save a Solidworks drawing as DWG (AutoCAD) format, it creates a separate DWG file for each sheet. That allows you to create separate part files for your system and still maintain a single model file for the entire weldment.
2) When you save a Solidworks drawing as PDF format, you can select which sheets you want to export. If you select only one then the PDF file it creates is only one sheet.
Either way I would do everything I could to maintain the integrity and accuracy of a single SW file for a single part.
RE: Ballooning a weldment with hidden parts
Can you explain how you are naming the different parts? The main reason I prefer working with independant files for each part/body is that I can have a separate file name for each part and the drawing keeps this same file name. It also prevents duplicate names.
I hope I'm not hijacking this thread though!
Patrick
RE: Ballooning a weldment with hidden parts
Scott Baugh, CSWP
FAQ731-376: Eng-Tips.com Forum PoliciesGryphon Environmental
www.2gryphon.com
www.scottjbaugh.com
RE: Ballooning a weldment with hidden parts
I have never felt a need to "name" the various parts of a weldment. We do fine with items 1,2,3, and so on as the Cut List automatically assigns them. If there are no names, then there also no duplicate names. If a need arises to refer to one particular body in a weldment we would probably just call it something like "Carriage Support Frame Weldment, Item 43".
The Cut List Properties dialog box has preset property fields (according to the template you use for that). You can add/edit those fields as you wish, thus giving you the ability to tie a "name" to each body in a weldment if you wish. That still keeps it all in one single, stable, and always up-to-date file.
I would highly recommend that you begin slogging your way through the learning process on creating and editing non-merged bodies, better known as weldments. It can be a little "less than user friendly" at times, but if you hang in there the result at the end is extremely useful and efficient. You will be glad you did it.
RE: Ballooning a weldment with hidden parts
Patrick
RE: Ballooning a weldment with hidden parts