Thicken/Offset not working Inventor 2017

[Anonymous]

Hi all, 

I'm trying to use the Thicken/Offset feature on a heatsink I need to include in my design. I have taken the .stp file from the manufacturer and I'm trying to make it bigger for a FEM simulation I need to do later on.

However, when I try to thicken the surface I get the following error message:

The attempted operation did not produce a meaningful result. Try with different inputs.

I have attached the file I have a problem with (sk441.stp). If I try using another heatsink profile everything works well. The geometry of the file that works, la_7.stp, is simpler, though.

Would anyone know a solution to this issue? Thanks in advance.

[mcgyvr]

How much were you trying to thicken it?

That error is just indicating it has a problem with one or multiple faces.. you should be able to select faces a few at a time and find the problem area then you may need to manually extrude or whatever..

You can also create a sketch on the profile of it and project all the edges then offset then extrude.. Its a fairly complex sketch/part though so I'd suggest doing it in small sections and maybe creating patterns or whatever to achieve what you need..

[Anonymous]

I tried 100mm first and then 1mm but the results is the same. I did forget to mention that I managed to extend it by projecting, creating a surface, extruding and then deleting the surface so I am left only with one body. I somehow did find a way to go around the problem but the Thicken/Offset was the most straightforwad way to do it and that's why I wanted to use that one.

[JDMather · Accepted solution]

Create an offset workplane 5mm from XY plane into the part. (drag above the solid body in the feature tree)

Right click on the body and select Solid Edit.

Select Extend/Contract Body.

Enter the amount to Extend (for 100 since it is already 10, enter 90)

Ping @johnsonshiue you might want to take a look at this one.  I tried other direct edit tools and they did not work.

Tried Replace Face, tried several things and Extend Body was the only technique that worked in my quick trial of the usual techniques.

[Anonymous]

Perfect. Thanks!

[johnsonshiue]

Hi Guys,

JD is right. This is a bug in modeling operation, possibly offset or Boolean. I will work with the project team to understand the behavior better. There is another alternative workflow without using Solid Edit environment. For this particular case, you can use non-uniform scale. Go to Direct Edit command -> Scale -> select the body -> set type to Non-Uniform -> Y direction = 50 or something -> Ok.

Many thanks!

[Xun.Zhang]

Just a quick update, ticket INVGEN-13016 was followed from now on.

Thanks!