Extruded Cut - "Failed To Merge Bodies"?

[Ballfreak10]

Hi all,

In the attached file, I'm trying to create a cut feature. Specifically, I'm looking to use the sketch "SKETCH Cut" to make a cut, up to surface, to "Cut Plane". I also only want the four outer contours selected, as shown in the screenshot. However, when I try this, I get the error in the screenshot.

Any ideas as to what might be causing this? All help is appreciated !

Thanks in advance,

[Glenn Schroeder]

When I tried the Extruded Cut without selecting contours I got this message,

which led me to believe there was something wrong with the sketch, and probably overlapping lines. Rather than trying to track it down I decided on another workflow. I edited the sketch, deleted all the exterior lines, and added relations to fully define the sketch.

Then I selected the "Flip side to cut" option in the Extruded Cut's property manager and it worked just fine.

[mike miller]

There are several problems.
The cut sketch has multiple intersecting profiles. If you only want to use the outer profile, why do you have an inner one? Wouldn't one be better? Actually, what's the purpose of the cut in the first place if you're going to remove the body you just made?
Also, the tree is very convoluted. It could be done with three features (or one, if you're doing what I think you are), and no extra planes. This doesn't hurt now, but it will later.

[matt]

Hi all,

In the attached file, I'm trying to create a cut feature. Specifically, I'm looking to use the sketch "SKETCH Cut" to make a cut, up to surface, to "Cut Plane". I also only want the four outer contours selected, as shown in the screenshot. However, when I try this, I get the error in the screenshot.

Any ideas as to what might be causing this? All help is appreciated !

Thanks in advance,




image.png

You have to learn how to make sketches that the software likes. It wants to see sketches where the action (cut or extrude or whatever) is performed by the solid lines, and anything else is the centerline/construction line type.

Also, it wants to see single closed loops of sketch entities that touch end-to-end without gaps or overlaps.

And a third thing it wants is for no infinitely thin knife edges. If you cut the canoe shape out of the block, in the middle of the block are two edges that are 0 thickness. In this case it works, but it may be giving you something you don't expect to see (the two bodies are cut into 8 bodies).

[mattpeneguy]

It is often quicker and easier to just create the geometry from scratch and 'get 'er done.

But, I also think there's a value in learning how to fix the problem, even though sometimes it takes more time, because one day you are going to discover a broken sketch at the top of the feature tree that you have to fix without deleting. So, @Ballfreak10 I recommend you try fixing your sketch with "Repair Sketch":