Extrude Hole – No target body found to cut or intersects

[kevinwatts]

I am trying to follow the tutorial, extruding holes through a body. As instructed I have set up construction line of axis and radius and centered a hole on their point of intersection.

https://www.youtube.com/watch?v=apkUQKNwHIo

When I say OK to the Extrude dialogue box the following message is given and no hole is created:

* No target body found to cut or intersects

Please tell me, what am I doing wrong?

[jeff_strater]

Sorry you are experiencing problems with this tutorial.  Would it be possible to post the model you are working with, or even just a screen shot of it?  Most likely the problem is easily solved, but I'd need a bit more info to be able to direct you.

Thanks,

Jeff Strater (Fusion development)

[kevinwatts · Accepted solution]

Hi Jeff,

I was able to over come this with trial and error. I will have to update this post for the benefit of others when I when I can figure out what I did right.

Have noticed that when extruding using a circle on the Plan I have to CTRL + select the circumference of the circle first, then select CREATE --> EXTRUDE, then reselect the hole circumference a second time.

Regards,

Kevin

[Anonymous]

I'm having the same issue.  Using extrude to cut and modify bodies.  Suddenly, the mode has completely quit working.  If I make a new body I can modify it but all the previous bodies it can't find.  All of my saved sketches behaving the same, some mode switch with fusion.  I don't have alot of time into this software, may need to try something else.

[Anonymous]

Hi,

I have this same "No target body found to cut or intersects" error issue when I try to extrude holes from two different sketches. I have extruded holes before, but it is not working now. I may be having a memory issue with my Macbook, because it only has 8Gb of RAM. My model is attached, and the issue is with the last two sketches.

8-Dale

[jeff_strater]

Hi @Anonymous,

I was able to get this to work with your model.  See this screencast:

You will notice in this screencast that I had some problems selecting the holes.  I don't know if you ran into this as well.  Part of the problem is that the sketch plane itself is a profile, also.  So, in this version, I start off by making just one curve a construction curve, which turns off that big profile, which makes selecting profiles much easier in this version:

Hope this helps,

Jeff

[Anonymous]

Hi,

I have been watching the screencasts many times. It goes so fast that I can't see what is going on in it. I wisg there was a way to just step through it. Sorry.

8-Dale

[Anonymous]

Hi,

I am having this same issue. I sketched a circle to extrude -cut on an already created body and I get this error, I also tried to use hole command and I am getting the same error. What is the reason for this error message? I can't seem to figure out the problem

Thanks

[Anonymous]

I have the same problem. I have tried creating an original sketch and using that. I have tried extruding and creating a sketch on the surface (along with the requisite points) but neither seems to work. Keep getting the same error message, "No target body found to cut or intersect".

UPDATE:  *** CORRECTION ***

It works okay if I create a top sketch (a sketch on the top surface of my extrusion), select the points and then click the little 'Flip Direction' checkbox on the 'Holes' dialog.

LAMENT: I wish this could be fixed to work from my original sketch on the bottom. That way I only have to draw one sketch instead of multiples.

(But, that said, the holes DO look very nice and the "Hole" tool is a very useful feature!!)

[TheCADWhisperer]

---

@Anonymous wrote:

LAMENT: I wish this could be fixed to work from my original sketch on the bottom. That way I only have to draw one sketch instead of multiples.

File>Export and Attach *.f3d file here that exhibits this behavior. I keep seeing this "issue" posted, but nobody supplies a file that exhibits the behavior.

[Anonymous]

Here is one that I just created with one sketch. If I use the hole dialog as it comes up the (with the direction checkbox checked) the holes are created correctly-- but on the back of the plate.

It I uncheck the checkbox, I get the no intersecting body error.

This is not the file that I used earlier but it exhibits enough of the problem that I think you could look at it.

I think the answer is going to be that the reason it works is because with the direction checkbox checked it inverts the sense of the holes and the body is in the correct relation.

Alternately if you extrude the sketch in the opposite direction (a negative direction) it works fine with the checkbox unchecked but not when it is checked.

EDIT -

I like this hole feature, but I wish it would work in the direction I am looking at the sketch *down* by default **UNLESS** I check the checkbox. I am fine with the checkbox inverting the sense of the holes. That's a useful feature. But it should start out by working *down* and I think that would probably eliminate most people's confusion.

[jeff_strater]

@bratwiz - here is a video that attempts to explain how Hole works with sketch input.  The rule is:  The default Hole direction is opposite of the sketch normal direction (which is opposite of the default Extrude direction - along the sketch normal).  For sketches created on solid geometry faces, the normal always points away from the material.  This gives consistent (and IMO correct) default behavior for Hole and Extrude.  However, if the sketch is created on a work plane (including the origin planes), the sketch normal is somewhat arbitrary.  The default for the origin XZ plane, for instance, is along the positive Y axis.  So, if you create a sketch on this plane, and the material you have created is above the XZ plane, the Hole default will be in the "wrong" direction.  But, if the material is along the negative Y axis, then the hole will be in the "correct" direction.

video:

[Anonymous]

Thanks for your reply. Now that I know I can adjust my expectations accordingly.

John

[LevitateGamer]

I need help with this problem of Extruding a Hole saying No target body found to cut or intersects

[jeff_strater]

@LevitateGamer - need more information - video, model, etc.  Cannot help you without that information.

[LevitateGamer]

Hear is what I am seeing

[jeff_strater]

can you post the model here?  Hard to tell from just an image.

[LevitateGamer]

Sure!

[LevitateGamer]

put it on the back of the distribution plate on the corners of the center rectangle

[jeff_strater]

@LevitateGamer - see message 12 in this thread for the detailed explanation of how Hole works with sketches.  In your case, that sketch was placed not on the face of the body, but on the XZ plane.  Because of that, the sketch normal is not away from the body, as it would be if you had sketched on the solid face.  Instead, it points in the opposite direction, so the default hole direction is not into the material.  There is a flip button on the hole UI specifically for this purpose:

screencast: