topic Re: help with curved rotated extrusion in Inventor Forum

help with curved rotated extrusion

rush02112 — Mon, 26 Jun 2017 21:42:52 GMT

Unless someone can show me otherwise, I know it is impossible to model the removal of material by a cylindrical objects (i.e. the path of a mill), but I am still needing to model something that is as close to the real thing. I have suffered trying everything I could think of to get this to work and all I have done is wasted time with this.

If you look at the attached model, I have 4 slots running parallel on the OD, 30 degrees apart from each other. I need to model the path a 0.419 mill slot going from 1 slot to the next.

Also included is the flat pattern, the 3d model currently has 4 slots starting from the left of the flat sketch file.

Re: help with curved rotated extrusion

johnsonshiue — Tue, 27 Jun 2017 01:18:01 GMT

Hi! Inventor is not yet capable of sweeping a volume as a profile. The closest thing Inventor can offer is Guide Surface Sweep cut. You will need to wrap the path around the cylinder and then use a rectangular profile as wide as the cylinder diameter. Then create a Sweep cut feature guided by the cylindrical face. I can show you an example tomorrow or you can do a search for Guide Surface Sweep to see how it is done. Again, this is just an approximation, not an exact cut resulting from a cylindrical tool cutting along a path.

Many thanks!

Re: help with curved rotated extrusion

rush02112 — Tue, 27 Jun 2017 04:05:22 GMT

I'm familiar with that technique. My only remaining question is should the profile be perpendicular to the axis of the part or perpendicular to the path around the cylinder? If I had to guess I would say perpendicular to the path.

Re: help with curved rotated extrusion

johnsonshiue — Tue, 27 Jun 2017 04:16:59 GMT

The profile should be positioned at a workplane normal to the path at the start of the path. The orientation of the rectangular profile should be aligned with a workaxis normal to the cylinder at the start point. So that, the tool is pointing to the normal direction on the cylindrical face.

Many thanks!

Betreff: help with curved rotated extrusion

WHolzwarth — Tue, 27 Jun 2017 13:47:21 GMT

I think, it's looking like that (2018 IPT)

Betreff: help with curved rotated extrusion

rush02112 — Tue, 27 Jun 2017 16:38:58 GMT

Walter,

Seeing what you did makes me realize how much more I have to learn with this software. In our day to day usage, I never have a reason to use the tools you used in this example. Matter of fact, my attached solution to this looks like a hack and slash job compared to your results!

Johnson,

With Autodesk offering CAM solutions, shouldn't removal of material by the path of a solid be added? If a customer were to need to do this type of modeling, wouldn't it also be impossible to generate correct G-Code from the model?

Betreff: help with curved rotated extrusion

rush02112 — Tue, 27 Jun 2017 17:00:18 GMT

To anyone else reading this thread, please go upvote the idea suggestion from 2014 regarding these type of issues!

https://forums.autodesk.com/t5/inventor-ideas/new-feature-sweep-solid/idi-p/5333169

Betreff: help with curved rotated extrusion

WHolzwarth — Tue, 27 Jun 2017 18:25:53 GMT

Dont expect too much from IdeaStation; it seems more like being a lottery.

I've seen entries there with only 6 votes being selected for future consideration. The one you mentioned has more than 450, but is still gathering support.

Betreff: help with curved rotated extrusion

rush02112 — Tue, 27 Jun 2017 19:09:28 GMT

and that is the sad part about it really...

I rebuilt my model using your workflow and I was able to deconstruct your process for making the paths work and understand it. Thank you again for showing me it to me. Being self taught only except for the occasional youtube guide, it's refreshing to look through someone's work for modeling outside of my norm.

Attached is my finished part if you care to take a look.

Betreff: help with curved rotated extrusion

WHolzwarth — Tue, 27 Jun 2017 19:21:52 GMT

That's looking very good, Aaron. Congratulations.

The shape coming out from real machining is still more complex, but by now, this is State-of-the-Art with Inventor's capabilities.

Betreff: help with curved rotated extrusion

johnsonshiue — Tue, 27 Jun 2017 20:32:40 GMT

Hi! I am not very familiar with HSM so I cannot make intelligent comments. But, I think creating Brep-geometry is one thing, while generating G-code is another. HSM generates perfect G-code but the geometry created by the tool is still based on Inventor API, if I understood it correctly. If Inventor could not do it, I am not sure how HSM would create such geometry.

Anyway, the ability to sweep a volume is one of the most frequent request. Inventor team is working on a solution which will offer more realistic geometry compared to our competitors. If you want to learn more, please sign up Inventor Beta program (https://bit.ly/InventorBeta).

Many thanks!

Betreff: help with curved rotated extrusion

WHolzwarth — Tue, 27 Jun 2017 21:04:48 GMT

Johnson, I'm still learning with HSM. But as I'm looking at HSM right now with my limited knowledge, it seems to me, that HSM only can follow pre-defined geometries.

In this case, these geometries are not existant from the beginning. What can HSM do here?

My impression: This is a task for a 2 (+1)-axis milling.

1st axis: Rotation of cylindrical workpiece around it's center axis

2nd axis: Movement of mill along Workpiece axis, or vice versa

+1 axis: Can be seen as feed relative to workpiece center.

Let's move now to Beta

Betreff: help with curved rotated extrusion

johnsonshiue — Tue, 27 Jun 2017 21:42:27 GMT

Hi Guys,

I have played around with this case a bit and I think there is probably another way to do this. Sheet Metal Unfold/Refold may help in this case. Take a look at attached part, I manage to convert it to a Sheet Metal part. I use Thicken feature to create a separate body. Then rip it so it can be unfolded. It should be fairly straight forward to create the connecting channels in the unfolded mode. Then you can refold it back. Would it work?

Many thanks!

Betreff: help with curved rotated extrusion

rush02112 — Wed, 28 Jun 2017 00:17:57 GMT

I will take a look at it when I am back in the office tomorrow. But the fact remains that we're only able to make an approximation. I don't need this functionality in inventor very often, but I would imagine the ~500 from the idea station do plus the countless others who do not come to the community site. I would like to know if you can put this in someone's ear for a future (2020?) software update. I understand this is more than likely a complex problem on your side otherwise it would have more than likely made it into a final build by now.

I have not used HSM any but we do have a copy of fusion 360 which has CAM built in. I have not looked to see if fusion has the capabilities we are looking for simply for the reason there is no vault functionality with fusion 360...

Betreff: help with curved rotated extrusion

johnsonshiue — Wed, 28 Jun 2017 01:13:20 GMT

Hi! Although I am not an expert on Fusion 360, I am certain the ability of sweeping a volume is not available there either.

Many thanks!

Betreff: help with curved rotated extrusion

WHolzwarth — Wed, 28 Jun 2017 12:24:51 GMT

I've tried to simulate the groove milling with Inventor HSM Ultimate; perhaps it's moving with HSM Express, too.

Generally, HSM showed problems with following the existing grooves in the transition zone.

And worse, there seems to be a bug: The mill is cutting deeper into the side faces than it should. Stopping at the end fillets seems ok.

See Mp4 Video in Zip, and attached sample file.