Possible to make a split bodies or cut in motion?

[yoshimitsuspeed]

In an assembly would it be possible to do a split body type action but in motion as one part passed through another? 

I can't really say much about the project I am working on so I'm trying to think of another applicable situation. 

Let's say the driveline components for this train sat directly below a structural beam and you wanted to remove the absolute minimal material as possible from that beam while allowing the drivetrain to spin unobstructed. So I am imagining a way to apply a split bodies command that allowed you to put it through it's range of motion and any material that was contacted in that range of motion would be made a separate body that you could delete. 
Would there be any way to do this in one clean sweep in F360? I know you could do it in steps moving a little then splitting the body and moving a little more to do it again but this would leave a very inaccurate and rough surface. 

[yoshimitsuspeed]

Forgot to post the link. 
https://www.youtube.com/watch?v=2n8uh-DBLFg

[lacrimacz]

I am not sure split body is the right tool to remove material. To me, it sounds like combine/cut would be more appropriate.

Just an idea: create a face, representing the cross section of the rotating part. Then a curve, representing the path of that part while rotating. The revolve or sweep to create a tool body and combine/subtract this body from the original part.

[yoshimitsuspeed]

Like I said this is only an example to show what I am trying to do. Not what I am actually trying to do. Naturally I can approximate the cut I need to make but it woudl be much better to remove the material from the actual path it makes minimizing the material removed as well as the possibility that some material might still be in the way. 
I am not looking for workarounds to achieve something similar. I am wondering if there is a way to remove material using the actual motion of the assembly. 

[lacrimacz]

You cannot rotate a body/assembly to remove material from other parts.

However, the steps I describe will not produce just an approixmation. They will remove exactly the volume needed. Your „actual motion of the assembly“ will be performed - when rotating/sweeping the cross section. As long as the cross section is the actual cross section and the path is the actual path, then the volume of the toll body will be *exactly* the same as the volume occupied by the part while rotating/moving.

[yoshimitsuspeed]

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@lacrimacz wrote:
You cannot rotate a body/assembly to remove material from other parts.

However, the steps I describe will not produce just an approixmation. They will remove exactly the volume needed. Your „actual motion of the assembly“ will be performed - when rotating/sweeping the cross section. As long as the cross section is the actual cross section and the path is the actual path, then the volume of the toll body will be *exactly* the same as the volume occupied by the part while rotating/moving.

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Well first of all even on a simple example as I used there will be complex curves that would be insanely difficult to make sure were absolutely perfect. You also have different diameter sections so some would take out a larger diameter cut in areas so you would at least need to take a few cuts but it would still be an approximation. Everwhere there is a corner passing through the cut if that corner has a chamfer, fillet, or complex shape it will change the shape of the cutout. 
More importantly in my case there are two objects in motion so while technically and theoretically there is a path that exists it would be rediculously hard to figure out what that path was and again it would be an approximation. One of the objects is tapered and enters the other object at an angle as the other object is moving up and down so a profile and path alone would not perfectly capture the shape of material removed. Again it would be an approximation. 

[yoshimitsuspeed]

The more I think about this the more I realize how far off a sweep would be to the actual shape. Not only would things like the shape of the leading and trailing edges affect the shape of the cut but there is also the fact that things like the connecting linkages on the train are not generally perpindicular to the path of motion. On a round object this would cut an oval path but in the areas where it was perpendicular to the path it would cut a round path. A sweep is only capable of staying perpendicular to the path or paralel with it's profile. Neither would cut the proper profile along the entire path. As I said before it would be no easy task trying to reproduce this perfectly with another means. 

[yoshimitsuspeed]

I would love any input on this. Whether any devs think there might be any workarounds or current solutions or if anyone knows if this will eventually be possible and if so a ballpark ETA?

[innovatenate]

Is this a parametric design?

If so, it should be possible to take snapshots of the assembly in critical positions. This will allow you to capture the positional data of your design. It should be easy to base the geometry of the design moving forward in the timeline off of the previous snapshots, thereby insuring adequate and precise clearance.

Without seeing the model, it's hard to say how automated you could make this process. For example, could you just project sketch geometry from existing components/work features to generate the new geometry in a precise manner. Another possibility is to use the Interference Analysis to see if there is any volumetric overlap between existing bodies.

If you check out the below Youtube video around the 7:15 mark, @keqingsong starts a positional modeling process  as an example. He generates some slot geometry that will insure the cutting blade will completely recess in the handle.

https://www.youtube.com/watch?v=TOh1m4Yp4bk

I hope that helps. Let me know if you have questions.

[yoshimitsuspeed]

Here is an example that should hopefully capture what I want to do. It's a bit different than what I need to do but it should give you an idea of the challenge.
http://a360.co/1N6fmIq

If you pay attention to the path the revolve follows you will see it takes a quick deep plunge initially but then as the disk spins only a narrow slit would be required to clear it.
Now naturally I could just whack a big chunk out of the disk so it clears but the goal is to remove as absolutely little material as possible.
If I could just take that animation right there, make the anvil let's call it say .2mm bigger and then make a cut using the motion in the assembly the groove removed from the disk would be the exact size and shape I needed allowing .2mm clearance for the actual part.

[yoshimitsuspeed]

innovatenate any chance you have time to take a look at that model and let me know if you have any i...

[innovatenate]

Below is a sample using positional modeling/snapshots. Take a look at the projected sketches in Component2. From here you may be able to create a loft or use this geometry to cut out the material in a very precise way. 

http://a360.co/1kTNhOl

I hope that helps. 

Thanks,

[yoshimitsuspeed]

I was afraid that would be the the best current answer.
Any idea if an actual dynamic capability like this could be possible in the reasonable future?
Knowing absolutely nothing about programming it seems like it shouldn't be too hard to do this.

[innovatenate]

For this exact assembly and approach there is an algorithm to the solution:

1. Rotate CAM
2. Take a snapshot
3. Perform the boolean command to subtract one body from another
4. Rinse and repeat.

I think the difficulty with a new feature (dynamic boolean?) that does this "automatically" is centered around resolution.... How many decimal places or how much resolution do you need when position the assembly? Do you rotate the cam by .1 deg .01 deg or maybe even .001 deg to generate a smooth surface? Even at .001 deg's of rotation (a high resolution), the resulting surface that is generated might not be 100% smooth face. In fact, it would have at least 360000 edges in for each boolean subtract. 

What you really want is infinite resolution, so the face is perfectly smooth, but this take a lot of computing. Luckily, the this tool actually already exists in the form of a sweep or a loft, etc... 

It takes some pretty advanced math to predict how to smooth the geometry "in-between" the snapshots. The geometry ultimately will boil down to the relative path between the CAM and follower and the position of the profile of the follower/plunger thing. You can get all of this required geometry from the model currently with the current functionality, then use the traditional tools to try and replicate it. 

You may be able write a script for this using the API, then it would be easy to automate and get a higher resolution than this example (which was done manually with ~20 or 30 iterations). However, you still run the risk of never having a perfectly smooth surface, the size of the design may grow out of control with too many edges, and performance will slow. 

This seems like a fairly complex feature request to me..  Not even considering all the permutations of mechanisms out there....  

As for the future, I would recommend adding it to the ideastaion and seeing where it goes. Some tools that exist in Inventor like the trace capability in Dynamic Simulation, might be a bit easier to start with...

I hope that helps.

[yoshimitsuspeed]

Yeah any way you cut it anything that did snapshot cuts wouldn't be ideal.
I would see it being essentially the same as a sweep but just with a variable shape profile set by the geometry of the cutting part in relationship to the cut part. Or something like that.

It seems like it could be a very valuable tool.

It would be very, um "CAD redefined"

[yoshimitsuspeed]

What if we used the technology in place in CAM and CAM simulation?
It seems as though that already does pretty much what we are trying to do here.

[dzid_]

Your question is on top in google when looking for motion cut.

Repeat pattern can do it. In particular repeat of a body-cut feature along a path. 

similar 

[superfedoruk]

Yes, I also lack the tool to solve such problems. Here is a video on how you can solve this problem with existing tools, but this solution is very far from ideal (
https://www.youtube.com/watch?v=ge8pcSXinww

[TheCADWhisperer]

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@superfedoruk wrote:

Yes, I also lack the tool to solve such problems. 

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This can be done correctly with Autodesk Inventor Professional.

Correct tool for the job.

[MichaelT_123]

Hi Mr SuperFedoruk,

 Consider to have a peek at:

https://forums.autodesk.com/t5/fusion-360-design-validate/need-rollers-that-conform-to-cable/m-p/869...

https://forums.autodesk.com/t5/fusion-360-design-validate/cut-one-body-from-another-while-they-are-i...

... although as many have had said "There is no straightforward solution  for F360 Ultimate users".

Regards 

MichaelT