Ballooning a weldment with hidden parts

[Refract3d]

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!

 

[Jboggs]

Haven't tried this in weldments but it works well in assemblies. To attach a balloon to an item that is hidden in the view, first switch the view to Hidden Lines Shown. Then attach your balloon to an edge of the hidden part, place it, and switch the view back to Hidden Not Shown. The balloon remains attached to the edge of the hidden part.

 

[PatCouture]

Obviously not the answer you want to hear but you would have more options in the assembly environment. I've always disliked having to make drawings of multiple body in the same part. SolidWorks Team is trying to make it usable but to me it's not good enough. So I always make different part files.

Good luck

Patrick

 

[Jboggs]

"to me it's not good enough"
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.

 

[SBaugh]

You can always use the hide\show bodies tab within the drawings view properties. That's what I use to show which is to be assembled first and on down. I do a lot of sheet metal and weldments with my latest job.

Hope that helps,

Scott Baugh, CSWP
Gryphon Environmental

http://www.2gryphon.com

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[PatCouture]

Jboggs

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

 

[SBaugh]

You can setup the drawing to use just certain bodies and this works very well with Weldments. When you first add a view to the drawing you will see the option in the top of the property manager "Reference Configuration". Don't be confused by the title, because directly underneath is the button for "Select Bodies". Here you can specify which bodies you want to show. Click this button and it flips you back to the model, select the body you want to show and that is the body or bodies that appear in the drawing. You can make one weldment appear in each drawing or multiple ones, its up to you. As for the Sheet metal parts, my guess is this will work as well, if not then you will have to use the drawing view properties like mentioned above.

Scott Baugh, CSWP
Gryphon Environmental

http://www.2gryphon.com

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[Jboggs]

PatCouture:
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.

 

[PatCouture]

Jboggs

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

 

[SBaugh]

Under the Bodies folder in the part for a weldment you can expand that and right click the bodies folder and go to properties to edit the properties of each one.

Scott Baugh, CSWP
Gryphon Environmental

http://www.2gryphon.com

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[Jboggs]

"Can you explain how you are naming the different parts? The main reason I prefer working with independent 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 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.

 

[PatCouture]

Thanks for the explanation Jboggs, I will keep an open mind towards weldments but the main reason I like to have names for my parts is because most of the parts I design are built by subcontractor therefore it's a lot easier to manage with separate files.

Patrick

 

[Jboggs]

You have different subcontractors that each build separate parts of a single weldment? Seems overly complex to me. But even so, you can still have one subcontractor build Item 6 as shown on sheet 3. You can show only one part per sheet if you like and still keep it all in one single file. Try it.