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you can make this work with these settings:
model is attached
Jeff Strater
Engineering Director
you can make this work with these settings:
model is attached
Jeff Strater
Engineering Director
Accepted solution
Hi @Anonymous.
You can follow the @davebYYPCU ideia. If you have two separate bodies it will work (create the cylinder as a new body). Then Replace Face will work.
See F3D attached.
Hi @Anonymous.
You can follow the @davebYYPCU ideia. If you have two separate bodies it will work (create the cylinder as a new body). Then Replace Face will work.
See F3D attached.
A slight modification to @jeff.strater solution will give you what you want and maintain one body. Model is attached as well as a short Screencast.
John Hackney, Retired
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A slight modification to @jeff.strater solution will give you what you want and maintain one body. Model is attached as well as a short Screencast.
John Hackney, Retired
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Accepted solution
when the 2 bodies are created separate, and not allowed to join into a single body, both @jeff_strater's solution and @davebYYPCU's solutions work. As you can see from the file @LeonardoBN uploaded, you still have 2 separate bodies, and you need to add another "combine" feature.
I've seen a few issues arise when bodies are allowed to join at an intersection that has no cross-sectional area. In this case the first extrude touches the barrel at it's tangent. It's unclear to me why fusion even allows this condition. the second grouping of extrudes shouldn't have defaulted to a join with the first body.
Jeff-what are your thoughts on that?
off the solutions presented, those would be my preference. The issue I see with @jhackney1972 is that if the thickness of the barrel is subsequently changed, you'll have to remember to go back and change the value in the extrude also. (unless you put a parameter in there instead).
@Anonymous - I'm curious why you went through all the trouble with a 3 point plane when the origin plane was available to you at the exact same location?
In any case, MY solution would be to model it differently, starting with revolving a profile of the barrel instead. I like to put as much information in sketches as possible. It seems easier to me to change dimensions in a sketch than to have to find the right extrude to dig through and change a value there. This approach is slightly more work on the front end, but figuring out how to make changes to it a year from now will be way easier. You might also notice there are a few less features in the timeline.
https://knowledge.autodesk.com/community/screencast/97c8ba82-2b57-4a7b-86b7-d636f26a1d66
when the 2 bodies are created separate, and not allowed to join into a single body, both @jeff_strater's solution and @davebYYPCU's solutions work. As you can see from the file @LeonardoBN uploaded, you still have 2 separate bodies, and you need to add another "combine" feature.
I've seen a few issues arise when bodies are allowed to join at an intersection that has no cross-sectional area. In this case the first extrude touches the barrel at it's tangent. It's unclear to me why fusion even allows this condition. the second grouping of extrudes shouldn't have defaulted to a join with the first body.
Jeff-what are your thoughts on that?
off the solutions presented, those would be my preference. The issue I see with @jhackney1972 is that if the thickness of the barrel is subsequently changed, you'll have to remember to go back and change the value in the extrude also. (unless you put a parameter in there instead).
@Anonymous - I'm curious why you went through all the trouble with a 3 point plane when the origin plane was available to you at the exact same location?
In any case, MY solution would be to model it differently, starting with revolving a profile of the barrel instead. I like to put as much information in sketches as possible. It seems easier to me to change dimensions in a sketch than to have to find the right extrude to dig through and change a value there. This approach is slightly more work on the front end, but figuring out how to make changes to it a year from now will be way easier. You might also notice there are a few less features in the timeline.
https://knowledge.autodesk.com/community/screencast/97c8ba82-2b57-4a7b-86b7-d636f26a1d66
@laughingcreek has it correct - the problem here is the non-manifold geometry created when you have a plane that is exactly tangent to a cylinder. That infinitely small line where the two meet throws the modeling kernel off.
The solution here is to (as @LeonardoBN says), to start off with two bodies instead of one. That takes a few edits of features to get those two bodies completely separate. Then, you still have the tangency issue, but the offset plane helps with that. In the screencast below, I separate the cylinder into a separate body, then do a join extrude at the end to put them back together.
Jeff Strater
Engineering Director
@laughingcreek has it correct - the problem here is the non-manifold geometry created when you have a plane that is exactly tangent to a cylinder. That infinitely small line where the two meet throws the modeling kernel off.
The solution here is to (as @LeonardoBN says), to start off with two bodies instead of one. That takes a few edits of features to get those two bodies completely separate. Then, you still have the tangency issue, but the offset plane helps with that. In the screencast below, I separate the cylinder into a separate body, then do a join extrude at the end to put them back together.
Jeff Strater
Engineering Director
@Anonymous
Just thought I would have a go at this with a slightly different slant on it 🙂
Easiest way I have found to do this and similar jobs is to as has already been suggested have the block and the tube as two individual bodies.
1) Use the "Press/Pull" function to extend the face of the block nearest the tube by a small amount, enough to have the block top and bottom edges at or slightly inside the Tube. (About 6mm does it)
2) Now use the "Combine" function to use the Tube to "Cut" the block but remember to check the "Keep tool" box so you keep the Tube.
That`s it, done, fast and easy, the block is now cut with the radius of the Tube so it fits exactly to the Tube.
Only thing left to do is remove the 4 small bits of the block that are left inside the tube, just use the "Remove" function to clear them out, then if you do want the whole thing as a single body you can use the "Combine" function again to join them together 🙂 🙂 🙂
Didn`t know if you wanted the holes through the Tube so I left that for you to do/or not 🙂
Just another way to do it without all the effort, file attached 🙂 🙂
Regards
Rob
@Anonymous
Just thought I would have a go at this with a slightly different slant on it 🙂
Easiest way I have found to do this and similar jobs is to as has already been suggested have the block and the tube as two individual bodies.
1) Use the "Press/Pull" function to extend the face of the block nearest the tube by a small amount, enough to have the block top and bottom edges at or slightly inside the Tube. (About 6mm does it)
2) Now use the "Combine" function to use the Tube to "Cut" the block but remember to check the "Keep tool" box so you keep the Tube.
That`s it, done, fast and easy, the block is now cut with the radius of the Tube so it fits exactly to the Tube.
Only thing left to do is remove the 4 small bits of the block that are left inside the tube, just use the "Remove" function to clear them out, then if you do want the whole thing as a single body you can use the "Combine" function again to join them together 🙂 🙂 🙂
Didn`t know if you wanted the holes through the Tube so I left that for you to do/or not 🙂
Just another way to do it without all the effort, file attached 🙂 🙂
Regards
Rob
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