Odd part

[Morglisn]

We manufacture custom-fit insulation parts, and are hoping to use Solidworks sheet metal functionality to provide cutting patterns for odd parts.

I'm attempting to create a "box" of insulation, 1" thick, open at the top and bottom. The insulation is coated on the outside by 1/8" foil. One corner is butted, while the other three will be fitted together by a 45-degree groove. I'm not sure if I'm providing enough information for an answer, but we're looking to draw the box, and obtain a flat pattern for cutting (both the total lengths, as well as precise location for routing the groove in the material for the corners.

In case the extra info helps, when the insulation is flat, we'll be making routed V-grooves for the corners. When laid flat, the groove will be two inches across, tapering to a point where the insulation and foil meet.

I know this may seem a bit convoluted, but I appreciate any help.

 

[DetroitPickles]

Sounds like no problem, but what do you want? Someone to tell you it can be done (other than a SW VAR), or someone to do it for you?

Let me know.

 

[dhinners]

It sounds like all the bending will be happening in your backing material. Try modeling the insulation as either an assembly where the backing is a sheetmetal piece, or in a part add the insulation after the bends.

 

[DetroitPickles]

I was assuming the same as you did. The only thing I wondered about was if the insulation was bonded to the 1/8" thick foil before it was cut and bent...

Mr. Pickles

 

[Morglisn]

I was actually looking for tips on how to do it myself. I'm new to SW, and am having a bit of a difficult time with some of the techniques. And, yes, the material is bonded before it is cut and bent (difficult, but that's the way we do it).

Thanks for your tips, guys, I'll be working more on this today.

 

[TateJ]

So, you cut the flat pattern - bond the insulation - then cut a v-notch along the bends - then bend the flat sheet into a box.
Wait - that's not right...
The insulation comes to you bonded to a 0.125 sheet of foil. You cut the pattern - v-notch the insulation, then fold the box.
If the boxes are always similarly shaped - but vary in size/scale - you can ignore the insulation for the patterning. Then make some in-context insulation parts in an assembly - just to check your final product before cutting.
Let me know if I'm on the right track - I'll expound further as needed.

Consume mass quantities...
tatej@usfilter.com​

 

[Morglisn]

We do apply the adhesives onsite, but that's not important, I guess. Yes, you're on the right track, that's exactly what we're referring to. What my superiors were looking for is to draw the box shape, apply the cuts while the part is folded, then unfold it for a flat pattern AND the location of the groove centers (for cutting purposes).

Thanks!

 

[TateJ]

here's what I tried:
I made the foil box (0.125 thick). Unfolded it and made seperate configurations - DEFAULT & FLAT. Then I inserted it into an assembly and started making the insulation. I defined the first piece in-context to the box bottom surface - this worked great. Then I made another piece on one of the sides. Both pieces were 1.0 thick & drafted in at 45 deg. I made a DEFAULT & FLAT configuration for the assembly too. I hoped that the in-context defined insulation pieces would fold up with the foil box - nope.

Now I'm thinking that if your box shapes are simple enough - you can make the insulation boxes as seperate pieces and mate them in an assembly to the foil box. Use design tables to define each piece's dimensions to fit the foil box - in all it's configurations. Bada-bing badd-boom you're all done, it's Miller time.

I know it's rather tedious, but if your boxes are simple enough, you'll only have to do it once. Sound reasonable?

Consume mass quantities...
tatej@usfilter.com​

 

[dhinners]

You can use a SolidWorks envelope to solve your problem: try this (if you haven't already solved it) -

1) In your assembly, Insert>envelope>new, & select the assembly 'Front' datum plane. This will create an envelope with its 'Front' coincident to the assembly 'Front'. I recommend going back into the assembly at this point, and deleting the 'Inplace' mate, then adding the appropriate datum-to-datum mates required to fully define the envelope creation.

2) Select your envelope & edit part, then create your sheetmetal 'Box' with a sketch showing the metal as-bent, leaving a gap where there will be a butt joint. In other words, your sketch should be a simple rectangle with a small opening at one corner. (Remember to make the gap slightly larger than the thickness of your sheetmetal if you plan to extrude with the thickness 'inside'). You can then Insert>Sheetmetal>Base Flange as a thin extrude. Set your sheetmetal thickness to 1/8", choose direction, etc. & SolidWorks will create the bends for you.

3) Still in the assembly, editing your part, insert a sketch on a parallel (or same) plane as your base flange & sketch your insulation. Make sure to leave at least a small gap wherever you will actually have a groove or cut in your insulation. I tried this, and it worked if I only set the insulation thickness in one spot, then used symmetry. Also, it was easy to use the vertices at the bend radii to keep a gap. With a few lines of symmetry you can make this whole sketch with only a couple of dimensions.

4) Extrude this sketch as needed. Now if you select the 'Flattened' icon, you will get a flat sheet with centerlines showing the bend lines (Which double as the router lines) and all the insulation "lumps" still attached. You can use this part in a drawing to show the routing operation.

5) Now, create a new assembly, and insert that same envelope into this new assembly (as an envelope). You can then use the envelope to create in-context parts for the sheetmetal and insulation separately by converting edges, extruding upto surface, etc.

6) Finally, insert your metal/insulation assembly into your master assembly.

Benefits: You can set the mass properties if you are concerned about weight, since the parts will have their own densities. Also, the BOM can show the sheetmetal & insulation separately for quantity calculation.
Also, if done in-context, all parts will be parametric.

Drawbacks: That's a lot of work to get those results. Hopefully this example will give you other ideas of what you can accomplish with envelopes in SolidWorks.

Whew! I hope that all made sense to someone!