Assembly with Derived Parts as Template

[trumph]

We make compression molded parts with steel plates by placing the plates in a mold, adding the composition material, and then closing the mold to compress and cure the material and adhere it to the plate.

When making Inventor models of these parts, I start with a model of the plate, and then create a model of the composition material, as if the plate wasn't there. I then create an assembly of the two parts. I create a derived part by subtracting the plate from the molded material. I then create the final assembly with the derived part and the original plate. I have attached a diagram of this process.

Is it possible to set up a template of the final assembly to make this process faster?

Thanks,
Tim Rumph

[trumph]

I forgot to mention that I am using IV10.

Tim

[JDMather]

> I start with a model of the plate,
If I follow you don't need this step

> I then create an assembly of the two parts. I create a derived part by subtracting the plate from the molded material.
and don't need this step

Create your Molded Part.
Start a new ipt part file and Derive Component the Molded Part as Body as Work Surfaces.
Offset a workplane and start a new sketch of the plate.
Extrude To Next the Derived Work Surfaces or
Extrude and use Split with the Solid option.
Turn off the visibility of the Work Surfaces.
Create your final assembly.

By this method you are creating the Tool from the Finished Part. If you change the Finished Part design the Tool is automatically updated.

[trumph]

The geometry of the plate is more complicated than shown in the example, so it would not be practical to create the plate by a simple extrusion.

Thanks,
Tim

[JDMather]

>geometry of the plate is more complicated than shown in the example
Can you post a representative example?

See 5 & 6
http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm

[trumph]

I tried to post the file to the Customer Files group, but got the following message:

The content type of the file 'V-780243 R18.ipt' is not allowed.

It seems strange that an ipt file could not be posted to an Inventor group. Lacking that, attached is a jpg file showing a couple of our plates.

Tim

[JDMather]

>It seems strange that an ipt file could not be posted to an Inventor group.

In Windows Explorer RMB on the file name and select Send to Compressed (zipped) folder. Attach the *.zip file. They should probably put these instructions in the FAQ.

[trumph]

Here is the ipt file in a zip file.

[JDMather]

Can you post the all of the finished files created using your current method.

[JDMather]

I'm not sure what you need as the end result but this was my 1st try done without any intermediate iam file you described.

[trumph]

Here is the finished file. I've broken the link to the assembly file so that the part will open without the files it depends on.

Thanks,
Tim

[JDMather]

This is an easy one.
Create your molded part without the cut.
Derive the plate as Body As Work Surfaces into the molded file.
Do a Split with the Split Part option. (you might have to flip the direction - if it cuts the wrong side simply edit feature and flip)
Expand the Derived body and turn off visibility of the derived surfaces.
No intermediate iam required. In fact I would derive the initial sketch for the molded part from the plate. Everything should work really slick. I would work up a complete example, but I am using r11.

[trumph]

Thank you Dr. Mather! I just tried this out and it works very well, and cuts way down on the number of files involved. I think that you've saved me a bunch of time on these parts.

Tim

[JDMather]

At least I got something right this morning.