5 axis G code

[tdcambridge]

Will Fusion offer 5 axis toolpath creation in the future?   Thanks 

[carl_bass]

Yes. You can see some of the 5 axis functionality that's already in the solidworks version and just coming out in the inventor version. Our goal is for all three platforms to have the same CAM funtionality

[tdcambridge]

Thanks so you have a solidworks plug in which creates tool paths for 5 axis machines? What is the product name?  When will this be added to Ultimate? 

[tdcambridge]

I guess your saying Fusion 360 ultimate will have the power of HSMWORKS which includes 5 axis machining ?  Thanks.. Awesome that the CEO of Autodesk has time to reply to forum posts !

[fonsecr]

Just an FYI Fusion 360 already supports indexed 5-axis. What Carl refers to is 5-axis simultaneous support (all 5 axes moving at the same time). You can use the Tool Orientation feature on the Geometry tab to make 5-axis indexed toolpath.

Note that you need a 5-axis post to use this feature. 5-axis posts do require more work to set up. And for 5-axis simultaneous support your CNC needs to support TCP.

Will need to talk with the team first before I can say when simultaneous toolpath will be available in Fusion 360. I'll reply later on this.

[carl_bass]

Rene is totally right. I just used HSM inside of fusion to do indexed 5 axis cutting today. But I am looking foward to simultaneous 5 axis

[tdcambridge]

TCP is a function of the geometry of the machine? What about making tool paths for  Swivel Head  with a Rotary Table  and/or using a trunnion table  ? Is there a guide /tutorial   regarding this functionality in Fusion?   Thanks 

[tdcambridge]

Hi so basically asking if Fusion will support 5 axis to support a Hurco type machine with a rotating material axis and a swivel spindle ?  Thanks 

[fonsecr]

We do support these machines. The generic HURCO post has 5-axis support built in. It uses G68.2 for 5-axis indexing. The post still needs to be customized though because it will only output pure 3-axis code when you post processor 3-axis toolpath. This is the behavior so old HURCOs can still run the posted programs. But if you post indexed toolpath the HURCO post will automatically turn on use of G68.2. You need to check if your CNC supported the multi-axis commands: G68.2, G8.1/G8.2, G43.4, M141, and M200. If your CNC does not support these commands it cannot run simultaneous toolpath. It is still possible to do some compensation in the post to allow indexed toolpath but it would require you to have your G54 on the rotary axis intersection which is generally annoying.

[tdcambridge]

Hi I don't have a Hurco but want to build a 5 axis machine with a swivel head and a rotary indexer.  My current control USBCNC doesn't support these codes.  Are they necessarty for 5 axis control in this configuration?  Thanks 

1. G0  rapid positioning

2. G1  linear interpolation

3. G2  circular/helical interpolation (clockwise)

4. G3  circular/helical interpolation (counterclockwise)

5. G4  dwell

G10 coordinate system origin setting

1. G17  XY-plane selection

2. G18  XZ-plane selection

3. G19  YZ-plane selection

4. G20  inch system selection

5. G21  millimeter system selection

G28 move to park position 1, setup on variable page

G30 move to park position 2, setup on variable page

G33 Lathe, motion synchronized to spindle
G38.2 straight probe

1. G40  cancel cutter radius compensation

2. G41  start cutter radius compensation left

3. G42  start cutter radius compensation right

4. G43  tool length offset (plus) , tool X offset for lathe

G49 cancel tool length offset

1. G53  motion in machine coordinate system

2. G54  use preset work coordinate system 1

3. G55  use preset work coordinate system 2

4. G56  use preset work coordinate system 3

5. G57  use preset work coordinate system 4

6. G58  use preset work coordinate system 5

7. G59  use preset work coordinate system 6

1. G59.1  use preset work coordinate system 7

2. G59.2  use preset work coordinate system 8

3. G59.3  use preset work coordinate system 9

G61 set path control mode: exact path

G61.1 set path control mode: exact stop

G64 set path control mode: continuous

G68 XY rotation
G76 Lathe, threading

1. G80  cancel motion mode (including any canned cycle)

2. G81  canned cycle: drilling

3. G82  canned cycle: drilling with dwell

4. G83  canned cycle: peck drilling

5. G84  canned cycle: right hand tapping

6. G85  canned cycle: boring, no dwell, feed out

7. G86  canned cycle: boring, spindle stop, rapid out

8. G87  canned cycle: back boring

9. G88  canned cycle: boring, spindle stop, manual out

10. G89  canned cycle: boring, dwell, feed out

11. G90  absolute distance mode

12. G91  incremental distance mode

13. G92  offset coordinate systems and set parameters

1. G92.1  cancel offset coordinate systems and set parameters to zero

2. G92.2  cancel offset coordinate systems but do not reset parameters

3. G92.3  apply parameters to offset coordinate systems

1. G93  inverse time feed rate mode

2. G94  units per minute feed rate mode

1. G98  initial level return in canned cycles

2. G99  R-point level return in canned cycles

[fonsecr]

Ok. I thought you used a HURCO control from your last reply.

USBCNC doesnt have built-in support for multi-axis toolpath. So you need to keep the fixture zero (e.g. G54) on the rotary axis intersection. You can run indexed toolpath this way. Simultaneous toolpath would not be possible - at least you would have significant quality problems since the control wont compensated the XYZ during interpolation of the rotaries. This is what TCP (Tool Center Pointer compensation) means. Ie. the CNC will make sure to cut along the XYZ in the fixture zero (e.g. G54) while the rotaries are changing. Keep in mind that the XYZ will need to be different / compensated as the rotary/rotaries in the table change/changes.

[tdcambridge]

OK so an indexed tool path could be run this way with a swivel mount and rotary table (HSM could create the paths for this?). Sorry for my ignorance.

Is there a reference guide for this? Thanks

Sent from mobile

[fonsecr · Accepted solution]

You only have to pick a new Z-axis using the Tool Orientation feature on the Geomtry tab. This will give you 5-axis indexed toolpath. This is already supported in the current Fusion release.

Check out tutorial Tutorial 3 - 3+2 Machining in the manual:

http://help.autodesk.com/view/NINVFUS/ENU/?guid=GUID874102C0-A738-4A72-80D5-F34B1D180132

[tdcambridge]

Thanks I appreciate your help. One final question? I assume this is only available in Ulltimate?    

[fonsecr · Accepted solution]

Yes, Ultimate level functionality because it requires more post customization to support multi-axis.

[steveripplingerjr]

Can I use this 3+2 machining to use my 4th axis? I do not have  a 5th axis but would like to play around with 4th axis machining. 

[fonsecr]

Yes, you can do 4-axis indexing also. Just comes down to the orientations you pick in relation to the WCS in the Setup. The customized post will do the conversion to the 4-axis axis and will error out if you by accident try to machine in an unsupported orientation.