Community
Inventor Forum
Welcome to Autodesk’s Inventor Forums. Share your knowledge, ask questions, and explore popular Inventor topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Ball End Mill Sweep

45 REPLIES 45
Reply
Message 1 of 46
ndogg1080
3201 Views, 45 Replies

Ball End Mill Sweep

Is there a way to do a clean sweep that imitates the shape a ball end mill? I'm trying to create a path that has 90 degree bends and whose end product looks like it was cut by a ball end mill. If there's a way to avoid sweeping the straight areas and then revolving the corners, I'd be happy to know.

Thanks!
45 REPLIES 45
Message 2 of 46
JDMather
in reply to: ndogg1080

Something like this?

-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 3 of 46
ndogg1080
in reply to: ndogg1080

Could you please save in Inventor 2008 format?

Thanks...
Message 4 of 46
JDMather
in reply to: ndogg1080

No

-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 5 of 46
mcgyvr
in reply to: ndogg1080

and technically thats not the correct shape a ball end mill will leave. If you need that actual path/shape that a ball end mill will create you need additional steps besides a simple sweep.

see attached Edited by: mcgyvr on Nov 20, 2008 3:53 PM


-------------------------------------------------------------------------------------------
Inventor 2023 - Dell Precision 5570

Did you find this reply helpful ? If so please use the Accept Solution button below.
Maybe buy me a beer through Venmo @mcgyvr1269
Message 6 of 46
ndogg1080
in reply to: ndogg1080

Could you save in IGES or STP format?

Did you use the REVOLVE function at the corners?

Thanks.
Message 7 of 46
mcgyvr
in reply to: ndogg1080

Yes you need to do a straight sweep first, then revolve (cut) at the end of the sweep to get the rounded end, then another sweep perpendicular into the center of the revolve.

So 2 straight sweeps and 1 revolve to make a right angle.



attached is the step file


-------------------------------------------------------------------------------------------
Inventor 2023 - Dell Precision 5570

Did you find this reply helpful ? If so please use the Accept Solution button below.
Maybe buy me a beer through Venmo @mcgyvr1269
Message 8 of 46
JDMather
in reply to: ndogg1080

>...and technically thats not the correct shape a ball end mill will leave

Here is the result I got in another SoftWare that will allow swept cut of one solid body through another.

-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 9 of 46
ndogg1080
in reply to: ndogg1080

That's what I'm looking for. What software did you use to make that?
Message 10 of 46
SJShaw
in reply to: ndogg1080

Created this in Inventor 2008 using an extruded cut feature and a couple of fillets.

Steve
Message 11 of 46
mcgyvr
in reply to: ndogg1080

>
{quote:title=JDMather wrote:}{quote}

>

...and technically thats not the correct shape a ball end mill will leave

Here is the result I got in another SoftWare that will allow swept cut of one solid body through another.




Well that other software is not correct either. The shape/lines at the corner should form a "Y" shape and not a "V". Get out a ball end mill and see for yourself. The file I posted above is exactly what will be produced when a ball end mill runs through it. Edited by: mcgyvr on Nov 21, 2008 8:41 AM


-------------------------------------------------------------------------------------------
Inventor 2023 - Dell Precision 5570

Did you find this reply helpful ? If so please use the Accept Solution button below.
Maybe buy me a beer through Venmo @mcgyvr1269
Message 12 of 46
Anonymous
in reply to: ndogg1080

The shape a ball end mill leaves in material at the corners depends on how the tool path is programmed, in JD's example the cutter is rolled around the corners, how the exact toolpath will be generated varies depending on the machine tool and whether cutter compensation is used or not.
Message 13 of 46
HallStevenson
in reply to: ndogg1080

I get neither a "V" nor a "Y" using ProE
Message 14 of 46
mcgyvr
in reply to: ndogg1080

The OP requested 90 degree paths.

Cutter compensation has nothing to do with it. Cutter compensation is simply offsetting the tool to the left or right (or up or down for a horizontal path) from the programmed path.



CAD programs like inventor cannot duplicate the proper shape with a simple sweep because the profile for the sweep is 2d and set to follow the path so when it gets to a corner it locks the inside edge of the profile and revolves the profile 90 degrees. This is NOT real world. What I posted IS correct and the only shape a ball end mill will make when programmed to do a right angle path.



Why the other program that JD used did not show the correct path makes me think that even though he swept what looks to be a 3d profile I believe the program is still taking a 2d shape from that 3d "tool" and sweeping it identical to how Inventor does it. I would be curious to see if he didn't do a rectangle path and stopped the tool in the middle of the part will it leave a rounded shape at the end or square like inventor will.


-------------------------------------------------------------------------------------------
Inventor 2023 - Dell Precision 5570

Did you find this reply helpful ? If so please use the Accept Solution button below.
Maybe buy me a beer through Venmo @mcgyvr1269
Message 15 of 46
Anonymous
in reply to: ndogg1080

> 90 degree bends

?
Message 16 of 46
Anonymous
in reply to: ndogg1080

> the result I got in another SoftWare that will allow
> swept cut of one solid body through another.

Ok. Now my ears are pricked.
Since when does Solidworks have a swept volume function?
Link to an article or description?
Message 17 of 46
mcgyvr
in reply to: ndogg1080


What's your point? Thats not a 90 deg (right angle) tool path...Thats a tool path with a radius at the corners. and thats exactly how Inventor treats a right angle sweep path too. Notice how the resulting corners from yours and JD's sweeps are identical (and incorrect in the real world)

If you programmed that path into a cnc machine it would look different than what Inventor outputs as the resulting cut.

This is why all engineers/designers should spend time in a machine shop.



-------------------------------------------------------------------------------------------
Inventor 2023 - Dell Precision 5570

Did you find this reply helpful ? If so please use the Accept Solution button below.
Maybe buy me a beer through Venmo @mcgyvr1269
Message 18 of 46
JDMather
in reply to: ndogg1080

>Since when does Solidworks have a swept volume function?

Added in r2008. I defined my path at the side of the tool rather than the centerline of the path. I included a very small radius (.001mm) in the 90° corners of the path.

-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 19 of 46
Anonymous
in reply to: ndogg1080

OP: "a path that has 90 degree bends"
_________________________________________

wrote in message news:6077110@discussion.autodesk.com...

What's your point? Thats not a 90 deg (right angle) tool path...Thats a tool path with a radius at the corners. and thats exactly
how Inventor treats a right angle sweep path too. Notice how the resulting corners from yours and JD's sweeps are identical (and
incorrect in the real world)

If you programmed that path into a cnc machine it would look different than what Inventor outputs as the resulting cut.

This is why all engineers/designers should spend time in a machine shop.
Message 20 of 46
Anonymous
in reply to: ndogg1080

In that instance Pro/E is extending the surfaces to intersection.

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report