Inventor - Cannot Do A Revolve Cut On Curved Panels

[mickmac06]

Hi,

I'm having problems performing a revolved cut on some curved panels. I've attached a couple of images, image 1 shows the revolved cut, which works on the smaller panels but when I select the larger panels the revolved cut fails. I then created a patch and used this to perform a split/ trim solid to remove the unwanted material as shown on Image 2, again, this worked on the smaller panels but not on the larger panels. I've attached the .ipt in the hope that someone can work out why this isn't working. Sketch 21 is the revolved cut sketch.

[johnsonshiue · Accepted solution]

Hi! This is a very interesting design challenge. I think I would use a different approach. When the precise body geometry can be reused, I would use it as much as I can. I would not build other geometry to replicate the existing one. In your case, the Lofted Flange already generates the base faces, which can reused to create individual panels.

Please take a look at the attached part. It should be close to what you are looking for.

Many thanks!

[mickmac06]

Thank you @johnsonshiue,

Your workflow looks ideal and is exactly what I was trying to achieve. Can I just run a couple of things past you to make sure I have understood your workflow correctly.

Image 5 (attached) shows a surface which you have offset to be in the middle of the 1.5mm stainless steel. (I don't seem to have the 'OffsetSrf1' command on my ribbon, where would I find it?)

You then used the 'Combine' command to join the two halves of the stainless steel together.

The next command you used was 'Delete Face' and I'm not sure why you did this?

You then used the 'Split' command to split the surface into individual panels.

You then used the 'Thicken' command to create the panels.

Does that sound correct?

Thanks again,

Mike

[johnsonshiue]

Hi Michael,

I am glad to help. It was a fun exercise. As you have found out, it does require a few tricks to work out like this. The Offset Surface command is actually within the Thicken command (enable Surface output). I guess consolidating certain solid and surface commands was an attempt to simplify the workflows and reduce the number of buttons. However, it can be confusing to the users on where to find the surface commands.

Patterning the two solid bodies and combining the two is to build a tool body to split the offset surface. The Delete Face feature turns the solid into a surface. Then simply select the deleted face body as the split tool to cut the offset surface, as opposed to creating 3D wires individually.

The objective is to get the panels as easily as possible. Then the Thicken command will take care of the rest. The approach you took was very straight forward. Basically, you built the geometry when you need it. However, it duplicates the geometry imprecisely. The 3D wires may not be on the surface. The Boundary Patch surfaces and the stitched surfaces may carry some tolerance. These minor deviations can make the downstream modeling unnecessarily difficult.

Unless it is absolutely necessary, I would reuse existing geometry (or replicate the exact geometry like Offset) to the max. Avoid recreating geometry in a different way. Usually, it will keep the feature tree simple and easy to manage.

Many thanks!