topic Re: 5 axis G code in Fusion Manufacture Forum

5 axis G code

tdcambridge — Mon, 08 Dec 2014 02:00:21 GMT

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

Re: 5 axis G code

carl_bass — Mon, 08 Dec 2014 02:03:01 GMT

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

Re: 5 axis G code

tdcambridge — Mon, 08 Dec 2014 02:06:07 GMT

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?

Re: 5 axis G code

tdcambridge — Mon, 08 Dec 2014 02:13:47 GMT

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 !

Re: 5 axis G code

fonsecr — Mon, 08 Dec 2014 02:21:37 GMT

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.

Re: 5 axis G code

carl_bass — Mon, 08 Dec 2014 02:24:59 GMT

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

Re: 5 axis G code

tdcambridge — Mon, 08 Dec 2014 05:53:53 GMT

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

Re: 5 axis G code

tdcambridge — Mon, 08 Dec 2014 21:05:43 GMT

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

Re: 5 axis G code

fonsecr — Mon, 08 Dec 2014 22:22:12 GMT

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.

Re: 5 axis G code

tdcambridge — Mon, 08 Dec 2014 22:37:37 GMT

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

G0 rapid positioning
G1 linear interpolation
G2 circular/helical interpolation (clockwise)
G3 circular/helical interpolation (counterclockwise)
G4 dwell

G10 coordinate system origin setting

G17 XY-plane selection
G18 XZ-plane selection
G19 YZ-plane selection
G20 inch system selection
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

G40 cancel cutter radius compensation
G41 start cutter radius compensation left
G42 start cutter radius compensation right
G43 tool length offset (plus) , tool X offset for lathe

G49 cancel tool length offset

G53 motion in machine coordinate system
G54 use preset work coordinate system 1
G55 use preset work coordinate system 2
G56 use preset work coordinate system 3
G57 use preset work coordinate system 4
G58 use preset work coordinate system 5
G59 use preset work coordinate system 6

G59.1 use preset work coordinate system 7
G59.2 use preset work coordinate system 8
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

G80 cancel motion mode (including any canned cycle)
G81 canned cycle: drilling
G82 canned cycle: drilling with dwell
G83 canned cycle: peck drilling
G84 canned cycle: right hand tapping
G85 canned cycle: boring, no dwell, feed out
G86 canned cycle: boring, spindle stop, rapid out
G87 canned cycle: back boring
G88 canned cycle: boring, spindle stop, manual out
G89 canned cycle: boring, dwell, feed out
G90 absolute distance mode
G91 incremental distance mode
G92 offset coordinate systems and set parameters

G92.1 cancel offset coordinate systems and set parameters to zero
G92.2 cancel offset coordinate systems but do not reset parameters
G92.3 apply parameters to offset coordinate systems

G93 inverse time feed rate mode
G94 units per minute feed rate mode

G98 initial level return in canned cycles
G99 R-point level return in canned cycles

Re: 5 axis G code

fonsecr — Mon, 08 Dec 2014 23:06:06 GMT

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.

Re: 5 axis G code

tdcambridge — Tue, 09 Dec 2014 00:33:51 GMT

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

Re: 5 axis G code

fonsecr — Tue, 09 Dec 2014 16:26:13 GMT

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

Re: 5 axis G code

tdcambridge — Tue, 09 Dec 2014 16:55:46 GMT

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

Re: 5 axis G code

fonsecr — Tue, 09 Dec 2014 17:00:25 GMT

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

Re: 5 axis G code

steveripplingerjr — Wed, 31 Dec 2014 13:25:44 GMT

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.

Re: 5 axis G code

fonsecr — Fri, 02 Jan 2015 12:12:44 GMT

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.