Trying to Use Circular Pattern on a Thicken(Cut) Feature

[Anonymous]

So far, I used a 2D sketch to project a 3D sketch onto a rounded surface. Then I used Split --> Thicken/Offset to cut the sketch onto the surface. But now I need a pattern of 4 rotated evenly through the same surface, but the circular pattern function won't let me click on the thickened cut feature.

Attached is my file.

I am using Inventor 2017

[JDMather]

There are multiple issues.

Let's start here in Sketch2 - is this what you really really want?

(Zoom in the area of the red circle.)

[JDMather]

You cannot pattern a Split (parent of Thicken), but you can pattern a body.

So make the feature as a New Body, pattern and then Combine-Cut.

But a much easier way would be to Offset (or Revolve) and Extrude-Cut up to Surface.

An Extrude-Cut can be patterned.

[CCarreiras]

Hi!

There's some special features that can't be pattern, the split is deppendent from a 3d sketch, dppending from a 2D ketch, is a very partiicular situation and can't be patterned.

Gladly, we have other ways to do it.

Check the file attached.~~tip: why you have extrusion1 + revolution1?  You can do all in only one revolve operation!!

[lordsonvijay123]

Hi, I'm facing a similar issue too. So I made a hexagon on the face on a curved surface. I've used the project to 3D surface, then split the hexagon and later used the thicken/offset to make a it hollow. I did not use extrude because I don't want the same hexagon to be behind the curved surface. But now I can't use the circular patter as I'm getting error while executing it. Please do help. The ipt file is given below. Inventor 2019.

[lordsonvijay123]

Hi, I'm facing a similar issue too. So I made a hexagon on the face on a curved surface. I've used the project to 3D surface, then split the hexagon and later used the thicken/offset to make a it hollow. I did not use extrude because I don't want the same hexagon to be behind the curved surface. But now I can't use the circular patter as I'm getting error while executing it. Please do help. The ipt file is given below. Inventor 2019.

[johnsonshiue]

Hi! The solutions were provide by experts already (see above replies). Instead of making it Thicken Cut, use New Body  option (first one as a new body, followed by the other two as join). Then pattern the Thicken body. Lastly, use Combine Cut to remove the Thicken body.

Many thanks!

[lordsonvijay123]

Thankyou for responding. The thing is I've done it but I'm getting the same shape behind the surface. The thing is since its a curved surface, the shape behind should be different according to the curvature of the cylinder. So to do that I have to project the sketch to the 3D surface. But the projected sketch is recognized by the cursor and so I have to use split. Then I tried to extrude but it doesn't recognize the projected sketch. So I used thicken/offset option. But now I can't do the circular pattern with the part worked on. That is the issue I'm facing. Feel free to use my ipt file for reference. Please help. Inventor 2019

Front view

behind view. The back projection should be changed with the curvature

[johnsonshiue]

Hi! I think I know what you want. I don't think Thicken is the right command to use in this case. You want to protrude the projected hexagon in Y axis, right? Instead of Thicken, you need to use Ruled Surface command.

In Surface tab, find Ruled Surface. Select the 3rd option on the left -> pick the hexagon -> pick Y axis as the direction. Repeat the process for other hexagon. Pattern the Ruled surfaces. Lastly use Sculpt command and pick the Ruled surfaces as the tool to cut.

Many thanks!

[nathan_wostrel]

I have a solution, however I am unable to save the file as it appears you are using 2019 and I'm using 2022.  It involves making surfaces that will cut through the part, patterning them, stitching the surfaces together, then using the combine/cut to remove the area needed.  Let me know if you need help with this.

Autodest® Inventor® Professional 2022

64-Bit Edition

Build: 287

Release: 2022.2

[SBix26]

Is this what you are looking for?  Emboss has the option to Wrap to Face, and maybe that's all you need?  Or do you need the hexagons to taper evenly so they are regular hexagons on the inside surface?

The attached file is 2019 format.

Oh, and please fully constrain your sketches.  It's really annoying to work on unconstrained geometry.

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Sam B

Inventor Pro 2022.2.2 | Windows 10 Home 21H2