topic Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360 in Fusion Design, Validate & Document Forum

Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

TheCADWhisperer — Wed, 23 Nov 2016 19:32:39 GMT

Is there an Emboss (Inventor) or Wrap (SolidWorks) tool in Fusion 360?

(10 year old references attached)

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

Anonymous — Wed, 23 Nov 2016 22:32:53 GMT

Howdy from your friendly neighborhood Megan.

Unfortunately, there's no "emboss" tool in Fusion 360, but there is a way to do it.

Here's a video that does a good job about how to emboss in Fusion 360.

I hope that helps,

Megan Ganley

Fusion 360 Catalyst

Student Expert

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

TrippyLighting — Thu, 24 Nov 2016 01:12:52 GMT

Nope, unfortunately there is not.

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

TheCADWhisperer — Thu, 24 Nov 2016 16:01:42 GMT

@Anonymous wrote:

...but there is a way to do it.

Student Expert

@Anonymous

Either you did not take the time to read the attached supporting documents or you failed to comprehend the complexity of the real-world geometry.

I recommend that you read this thread and then take a look at the documents I attached to the original post.

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

TrippyLighting — Thu, 24 Nov 2016 17:19:54 GMT

I agree. This can be done, however it is definitely more wrk than wrapping a sketch around a cylinder. I'll create a screencast after I had my helping of turkey an Pumpkin pie 😉

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

scottmoyse — Thu, 24 Nov 2016 18:47:32 GMT

Well at least you can machine this type of geometry in Fusion 360 now, just not model it.

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

TheCADWhisperer — Thu, 24 Nov 2016 18:54:55 GMT

I always thought it interesting that we can animate tool paths (one solid removing material from another) but no modeling processes to do the same (the SWx process is very limited in functionality).

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

TrippyLighting — Thu, 24 Nov 2016 21:50:06 GMT

Here is one approach how it could be done in Fusion 360. I have a few others, but while a bit more work to set up, at the nice thing with this version is that al the basic parameters are accessible through the dimensions in the top 2 sketches. The other sketches in the attached file are simply there to provide the framework for the sweep feature.

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

JDMather — Thu, 24 Nov 2016 22:16:59 GMT

~~Can you File>Export the *.f3d file to your local drive and then Attach the file to a Reply~~.

Oops, I see that it is there. Back in a few minutes.

I do not believe that your "solution" results in the correct geometry - but you did give me an idea of how it can be done (with an inordinate amount of extra work) .

You can check your "solution" by adding a cylindrical follower and simulate the motion and check for interference.

Sweeping a rectangular profile does not result in the same geometry as sweeping a cylindrical cutter.

You might have noticed what seems like an inordinate amount of work in the documents that I attached.

Of course, I could use a full-feature engineering tool to generate the cam, but it can be good for the students to think about the geometry in-depth.

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

TrippyLighting — Thu, 24 Nov 2016 22:14:21 GMT

The .f3d is attached to my post 😉

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

TheCADWhisperer — Thu, 24 Nov 2016 22:53:51 GMT

I have to do a bit more testing, but from my initial testing, I think you did in fact find a correct solution.

Now... how do I change to different motion laws on the rise and fall....

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

TrippyLighting — Thu, 24 Nov 2016 23:18:05 GMT

Yeah, I've thought about that as well but would have to say that might be a bit more tricky than this one.

There is just so much you can do with a spline. Some profiles might be possible, others might not.

However, given how you created the geometry in the other thread with the knot (brilliant BTW), I could imagine that that a similar methodology could possibly be used to create the correct path for a specific motion profile.

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

michallach81 — Fri, 25 Nov 2016 10:09:59 GMT

Hi guys, I have to agree with Jeffrey (@JDMather). Peter's (@TrippyLighting) method is not mathematically accurate, here's an image with section at random angle (with axis on cylinders center, of course):

To be able to create certain geometries we need "wrap" tool ( I would like to use term roll/unroll to distinct from wrap/unwrap, developable surfaces vs non-developable surfaces), even more, we would need also solid sweep (sweeping solid body).

I was struggling with much simpler examples, like in this thread: http://forums.autodesk.com/t5/design-validate-document/wrap-a-body-around-a-cylinder/m-p/6246589#M50166 ,

where I succeed to get what was desired, but only because no one was asking to made "fillet" where cutter would start climbing. That exact problem have occurred in this thread: http://forums.autodesk.com/t5/design-validate-document/model-a-cut-around-a-cylinder/m-p/6269226#M51976 ,

and I terribly failed to find solution.

If you like to bend your minds, please try to create math accurate model (mine is attached below, it's the same as in thread I refer to).

Other thing is that we can get slightly better results in Parametric Barrel Cam model (another file in attachments), still I'm not convinced if path curve is correct. Even flat curve should be equation driven curve, not a spline.

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

TrippyLighting — Sat, 26 Nov 2016 13:17:04 GMT

@JDMather @michallach81 Very cool. You are correct, my first approach does not create the correct geometry. I marked Michal's answer as the solution even though it really is not a real solution to the original question whether there's a wrap function.

But in the end, that's what a Forum is for. Rational discourse and learning.

Actually I am also not sure if my spline approach creates a valid sinusoidal curve as well, but that's the best I could come up with 😉

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

marc7X3XJ — Mon, 28 Nov 2016 00:58:07 GMT

I really appreciate your screen cast on the Barrel Cam but I am missing something somehow. I can not figure out how to sketch the splines between the three planes? I am sure that it is probably something simple but I can not figure it out after spending hours trying. I am still finding my way around Fusion 360 and have no formal training. If you could point me to the right command I would really appreciate it.

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

TrippyLighting — Mon, 28 Nov 2016 01:04:59 GMT

Each of the splines is created in it's own new sketch.

You basically start new sketch and pick a plane. it will be a 3D sketch and what place you pick is irrelecvenbt, but you have to pick one. Than you can start sketching the spline.

in the Sketch Pallete I usually turn the "Sketch grid" off and "3D sketch" has to be enabled for that to work.

If this does not help you may want to prepare a screencast so we can see where the problem is.

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

marc7X3XJ — Mon, 28 Nov 2016 01:51:32 GMT

Thank you. That explained it perfectly. I was able to complete the sweep but now I need a little clarification on how to correct the edges of the cut to be perpendicular to the cylinder as it will be cut on a 4th axis.

Thanks again,
Marc

@TrippyLighting wrote:
Each of the splines is created in it's own new sketch.
You basically start new sketch and pick a plane. it will be a 3D sketch and what place you pick is irrelecvenbt, but you have to pick one. Than you can start sketching the spline.
in the Sketch Pallete I usually turn the "Sketch grid" off and "3D sketch" has to be enabled for that to work.

If this does not help you may want to prepare a screencast so we can see where the problem is.

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

TrippyLighting — Mon, 28 Nov 2016 02:06:46 GMT

User @michallach81 pasted an improved version. Roll back the timeline and see what he did to achieve the correct geometry.

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

marc7X3XJ — Mon, 28 Nov 2016 15:12:30 GMT

@michallach81 wrote:
Hi guys, I have to agree with Jeffrey (@JDMather). Peter's (@TrippyLighting) method is not mathematically accurate, here's an image with section at random angle (with axis on cylinders center, of course):

To be able to create certain geometries we need "wrap" tool ( I would like to use term roll/unroll to distinct from wrap/unwrap, developable surfaces vs non-developable surfaces), even more, we would need also solid sweep (sweeping solid body).
I was struggling with much simpler examples, like in this thread: http://forums.autodesk.com/t5/design-validate-document/wrap-a-body-around-a-cylinder/m-p/6246589#M50166 ,
where I succeed to get what was desired, but only because no one was asking to made "fillet" where cutter would start climbing. That exact problem have occurred in this thread: http://forums.autodesk.com/t5/design-validate-document/model-a-cut-around-a-cylinder/m-p/6269226#M51976 ,
and I terribly failed to find solution.
If you like to bend your minds, please try to create math accurate model (mine is attached below, it's the same as in thread I refer to).
Other thing is that we can get slightly better results in Parametric Barrel Cam model (another file in attachments), still I'm not convinced if path curve is correct. Even flat curve should be equation driven curve, not a spline.

I believe that I have followed you improved model accurately up until the split face. At that point I see that you split tool is from the sweep but I can not figure out what you selected or how you selected it. My test cam slot is slightly different because motion pauses for 72 degrees and I am no sure if that is making a difference or not. I will attach the test example.

Re: Emboss (Inventor) or Wrap (SolidWorks) in Fusion 360

michallach81 — Tue, 29 Nov 2016 07:23:50 GMT

like that: