Cancel
Showing results for 
Search instead for 
Did you mean: 

4 axis milling

Pioneer
Pioneer

I would like to use 4 axis to mill Outside profile. Which tool path it is suit for this part?

 

8 REPLIES

Re: 4 axis milling

variable contour, with 4-axis normal to part would be where I would start.  Or you could use sequential mill.

Jake Hardwick
CNC Programmer
Senior Aerospace AMT
Production NX8.5.3.3 Beta testing NX10.0.1.4

Re: 4 axis milling

Pioneer
Pioneer

I met this alarm when I use 4 axis normal to part. How to fix this? ThankS!

Re: 4 axis milling

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Guessing...

You have drive geometry but no part geometry?

I believe there is "4 axis normal to drive" option

You could also try "Away from line" and pick a line at the (approx) centerline of your part.

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: 4 axis milling

I see 2 ways to cut this in 4 axis.

Do you want to cut with the side of the tool or the end of the tool?

 

For the end, surface contouring is the way. You need to decide on what tool axis you want (away from line should give you the smoothest rotary motion) and if you want to project the tool on to the the part (select PART), or just follow the drive geoometry blindly.

 

To use the side of the tool, solid profile 3D or zlevel should do it. You may need a start event to lock an axis, so the part spins around, instead of the tool going around the part. 

Mark Rief
Retired Siemens

Re: 4 axis milling

Gears Legend Gears Legend
Gears Legend

Here's a sample.

Tool axis = 4-axis relative to part. This prevents rubing of material in the center fo the tool

Patrick Delisse
KMWE - DutchAero
NX 12.0, TC 11.2, CAMPOST V22, Vericut 8.1, TDM 4.8
C#, VB, .NET

Re: 4 axis milling

Pioneer
Pioneer

I try different way to mill this. But It is not work! Someone can help to take a look? I would like use Bull end mill to mill OD surface IN 4 AXIS, It is possible?

 

Thanks in advance!

Please see attachment!

Re: 4 axis milling

Gears Legend Gears Legend
Gears Legend

The problem you have is caused by the tool size in comparison with the part size.

With a tool diameter much larger than the part details you will need to specify

part geometry. This way NX can project the drive points onto the part and prevent gauges.

 

Set the tool axis to 4-axis Normal or relative to part if you need 4-axis output.

 

I would suggest a smaller tool. If you look at the toolpath (verify) you see that the part doesn't have a greate finish, even the scallopheight was specified at .0001

 

A better solution -to my opinion- is to use a fixed contour operation to machine a section and use transform > instance to go around

 

Patrick Delisse
KMWE - DutchAero
NX 12.0, TC 11.2, CAMPOST V22, Vericut 8.1, TDM 4.8
C#, VB, .NET

Re: 4 axis milling

Creator
Creator

 

Hello.

Thank You for  constant support to CNC Community.

I try to create Mill-Turn Post, but in order to do so, I need transfer some of the Variables from "Program Start Sequence"

in Lathe Post, to "Program Start Sequence" in Mill Post how I can efficiently do this?

Learn online





Solution Information