iProperties and a multi-body part don't work do they?

[guyh]

Maybe this is not the intended use or I'm not fully understanding the principles but if I make a multibody part and assign the solid bodies material properties the combined part does not have the properties of those materials in it's iproperties. I would think at least it would be able to give me the weight?

[PaulMunford]

A part file can only have one material. I think that you've applied different finishes to your different bodies, not different materials.

To get a combined weight you would need to create an assembly from your 'Master' Part file (Using the Create Components tool on the 'Manage' Tab). You would then be able to set each parts materials property and get the weight from the Assembly.

TheCadSetterOut.Wordpress.com

[Anonymous]

Create component from each individual solid and assign the material to newly
created part. When you create an assembly from all the parts - you will get
the weight of the assembly.
Regards,
Igor.

--
Web: www.meqc.com.au
www.boatworks.meqc.com.au
wrote in message news:6351958@discussion.autodesk.com...
Maybe this is not the intended use or I'm not fully understanding the
principles but if I make a multibody part and assign the solid bodies
material properties the combined part does not have the properties of those
materials in it's iproperties. I would think at least it would be able to
give me the weight?

[mflayler2]

You can also assign the material in the multi body part, but it will not carry through to the derived file. Kinda worthless, except for checking initial wt.

[Anonymous]

Especially if parts are going to have different physical properties.
Plastic, Bronze, SS steel in one assembly.
Igor.

--
Web: www.meqc.com.au
www.boatworks.meqc.com.au
wrote in message news:6352720@discussion.autodesk.com...
You can also assign the material in the multi body part, but it will not
carry through to the derived file. Kinda worthless, except for checking
initial wt.

[osaldivar_frisa]

Igor,

I am trying to make a multy-body solid using iPart table. I did it, no problem bbuutt the Make Components command is no longer available so I can't export the multi-body solids to an assembly and document it properly. I need to put the bodies into a drawing and document their mass separetely. Its so frustrating that it won't do it. I have also sought for a way to do it via API but there is no oBody interface, or is it?

Please help.

Omar.

[johnsonshiue]

Hi! Make Component is blocked when you are working on an iPart factory with multiple solids. It is because iPart member is already a derive part to the iPart factory. It does not make sense introducing nested derive relationship to an iPart member.

You can simply insert the member to an assembly just like any regular iPart.

I assume the reason why you want to use mutli-solid iPart is to create one solid per member, right? If each member needs a different material style, you can edit the author table->go to Other tab->create a new column->right-click on the header->check Material Column. Then you will be able to assign material to each member.

Thanks!

[osaldivar_frisa]

Johnson,

Thanks for your answer. Here's the complete picture:

1. We have many similar parts for which I wanted to use an iPart factory.
2. I want to control all dimensions and parameters via Excel. This way I can make changes easily even if changes are done over a large number of members. One more reason to gor for the iPart approach.
3. I need to output drawings in a very specific way: the outer and inner contours need to be shown.
4. In a conventional solid you can display intermediate sketches to depict the inner contour I mentioned above. Since an iPart member is a derived solid no construction sketches are available for display in the idw.
5. Because of (4) I used a multi-body member inside the iPart factory. Having two solids allows for the kind of sketch I need. It has the inconvenience that since the member is a multi-body I can't display the two object's mass separately in an idw.
6. Since one body is inside the other, and the mass I wanted to document is the one of the intersection, I made the outer body to be hollow. Then the sum of masses was correct and I could display it properly in the idw.
7. I had to create a parts list and embed it into the idw's title block because I couldn't add the desired field through a normal text box.

All this is in the files I attach to this message. I can work with this but would like to know if there's a simpler way to do it.

Thanks

Omar