Can you have more than one material in a weldment part?

[rammy17]

Hi

Just a quick question

I created a weldment part which has 3 layers created from one sketch on the side plane and extruding mid plane. The top and bottom are mild steel and the middle layer is rubber, is there any way of changing the material in the part without creating an assembly, the reason i ask this is because if the material is left as default then the weight in the drawing border will be incorrect.

Cheers

 

[handleman]

I don't believe SW has the capability of applying different materials to bodies of a single part.

-handleman, CSWP (The new, easy test)

 

[ctopher]

They have to be separate parts in an assy.

The weight/material should be indicated on the part description/drawing, not the assy...but the BOM for the assy.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

 

[alejandroillini]

think of real life you can't have a weldment with two different materials (typically) however you can assemble things into it before or after welding usually after

 

[NL8]

I would disagree alejandroillini. You could have multiple grades of steel, 1010 cold rolled, A36 structural, etc. going into the same part. All still steel, but with varying material properties that could affect the final outcome of weight or static analysis.

Joe Hasik, CSWP/SMTL
SW 08 x64, SP 4.0
SW 09 x64, SP 0.0
Dell T3400
Intel Core2 Quad
Q6700 2.66 GHz
3.93 GB RAM
NVIDIA Quadro FX 4600

 

[ctopher]

This is true.
I have actually modeled two different materials welded together. Both parts and the weld...3 different material properties.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

 

[brengine]

rammy17,

In a Part file, use the native SW Weldment tool. It will create a multi-body part. In the cutlist, you can independently define any material you want for each of the Items in the Cutlist. "Merged bodies" have to be one material (because they will appear as one Item in the Cutlist), so make sure to to Uncheck "Merge Result" when defining the feature.

Note, if you are Patterning or Mirroring, you must use the Feature Scope correctly when initially creating this feature. Make sure you choose correctly as far as if you are trying to Pattern/Mirror a Feature or a Body, because you can not later edit the Pattern/Mirror Feature and choose the other. You must delete the feature to change the scope from Feature-to-Body or vice-versa.

This really is the best way to make a Weldment, and SW really excels with this tool. Just make sure each "body" is an item that in the real word would have to welded to another "body". Periodically check your "Bodies" folder to make sure you're getting the separate bodies that you want.

Do not model components to their Machined size. The top portion of your Feature Tree should be the bodies in their "As Welded" state, and then add your Machined Features. Make sure to set up the "As Welded" and "As Machined" configurations to match your intent. If you don't, you may not be able to link the required dimensions for the Stock Material sizes, plus it could require a little more manual tweaking to get your Cutlist Quantities correct.

While in the "As Welded" configuration, assign properties to each Cutlist Item; like Material, Shape, parametrically link to dimension values, or whatever other property you want.

Once you're in the 2D Drawing, all you have to do is "Insert" a Cutlist Table based off of one of the views of your weldment in the "As Welded" configuration.

I hope this wasn't information overload. I can clarify more if needed.

Ken

 

[brengine]

rammy17,

Doh! I should've read the OP a little closer. Everything I stated was intended for creating a Cutlist on your drawing...I don't think you can apply multiple materials to a single part file.

As stated above...Do it as an assembly.

Ken

 

[DesignerGuy16]

You can do it as a "weldment" just save the seperate bodies out as parts, set your properties, then reassemble.

If master modeling is your thing, this is an acceptable solution to a solidworks limitation.

James Spisich
Design Engineer, CSWP

 

[overkill4]

Would creating each part individually then inserting into a single part file work as well?

Haven't had a chance to try that but I thought I'd put it out there.

60% of the time, it works every time.

 

[handleman]

Inserting a part into another part file brings its geometry in as a (mostly) dumb solid. Its material properties will not be brought in. A part file in SW can only have one material applied. Each solid body in the file will have the same material properties.

-handleman, CSWP (The new, easy test)

 

[takedownca]

I don't have 2009 installed, but I found this SPR in the list of fixes for SP0.0.

442679 Cannot apply or edit material on a single body of a multibody part as advertised

I don't have evidence it's actually true, but this implies that as of 2009 you can apply multiple material properties per part file.

 

[J-C]

It didn't make the cut for 2009.

Jason

SolidWorks 2007 SP5.0
SolidWorks 2008 SP0.1
WinXp sp2 (32 and 64 bit)

 

[arcticcatmatt]

Sure.. we run SW2007. In the cutlist in the part file you have a list of solidbodies. You can change the property of the solidbody you want to change to whatever you want.

 

[handleman]

The cutlist means nothing to the OP. He wants different materials with different mass properties, not just some text in a weldment cutlist property.

-handleman, CSWP (The new, easy test)

 

[arcticcatmatt]

^ I am an idiot.. I missed that in his post.
Sorry about that.