Problems with 'replace face' command

[Anonymous]

Ok I am having issues with the 'replace face' command. I have attached the part I am talking about. I drew a 2D sketch and engraved/embossed it on the part. Then created a surface that I want to replace the face to. If you look at the part you will understand what I am talking about. Now with the enraving being narrow, it works perfect. As soon as you widen the rectangular sketch to where the emboss takes up more of the part than the original outside OD, it removes all material inside the  created surface.

Any experts understand why this is or know how to fix it or get around this issue? I have a part that I need to do this on but the emboss is too wide and it does what I just described.

Thanks in advance.

Dave

Inventor 2013

[wilkhui]

Hi and welcome to the forum, Dave!

I'm not sure that I'm seeing the behaviour that you describe, would you be able to post a part file with the feature that isn't working as you'd like?

Perhaps this is unrelated but the sketch that you have used to Emboss results in non-manifold geometry - is this your intention?

Looking forward to your response,

Indy

[Anonymous]

I have attached the exact same part and renamed it. The only difference is I made the emboss sketch (sketch 5) wider than before. It seems that instead of replacing the face outwards to the selected surface, it moves the face inwards 'through' the part to the surface removing all material inside the selected surface. I am completely baffled.

And this was just a test part to show what I was trying to accomplish. That's the reason I didn't define any of the sketch geometry. This is to eventually be a complex extrusion screw for plastics processing. I tried to upload the actual file that I was working on but it was too large to attach, so I made this test part.

Thanks,

Dave

[JDMather]

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@david_reynolds wrote:

 I tried to upload the actual file that I was working on but it was too large to attach, so I made this test part.

Dave

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Find the red End of Part marker.
Drag the red EOP to the top of the feature tree hiding all features.

Save the file with the EOP in this rolled up state.

In Windows Explorer right click on the filename and select Send to Compressed (zipped) Folder.

Attach the resulting *.zip file here.

What is the purpose of the WorkAxis1?  Isn't it an unneeded duplication of the Z axis?

[Anonymous]

Thanks for the heads up on the saving issue. Didn't realize moving the EOP would reduce file size when saving.

The axis is there just because I was messing around trying other things. It's not needed.

Any ideas on the main issue JD?

Dave

[wilkhui · Accepted solution]

Hi Dave,

You're right, there are some improvements to be made here; I've logged this issue as DID 1491406 for future reference. Thanks for reporting this behaviour!

There's a workaround that hopefully isn't too intrusive - if you project cut edges and trim off the little piece of Sketch4 that sticks out of the bottom face of Extrusion1 then you should be getting the behaviour you expect:

Hope this helps and thanks again!

Indy

[SER4]

The wording in your reply helped me find a solution!

Use the SPLIT command to 'cut' the "To" surface in half...this way it will not replace the face to the 'other' side (e.g. other half of a cylinder).

[johnsonshiue]

Hi! Another helpful workflow is Delete Face -> Heal. This command remove an existing face and reintersect the adjacent faces. It helps repair bad or redundant geometry nicely.

Many thanks!