4th Axis, Machining Heights, WCS

[Anonymous]

HI All, 

I'm new to Fusion and CAM in general and I've been trying to find how to setup my rig. 

Let me describe my setup:

I have a three axis CNC mill with a 4th axis aligned with the Y axis.

Mounted on the fourth axis, I have a box on which I need to machine four faces. Box rotates and Z goes down and holes are cut.

I got all that figured out but I have difficulty in getting a reliable location for zeroing my G54. I initially designed the CAM setup to have a WCS zero on a corner of the box but when checking the G code I realized that the heights were calculated that point and not from the individual faces that are defined in the tool orientation. That was a little unexpected since these menus show distances according to these face coordinate systems... but anyways...

I kind of have a working setup now where if I put the setup origin on the rotation axis I have all the limits heights OK but now, I would have to zero from the middle of the piece which is quite difficult, as least given my current knowledge of things. 

So my question is, what is the best way to go about that? Should I keep the setup zero on the rotation axis and find an external way to find my G54 zero. Or should I try to find a way to get the limits and heights right with Fusion with an off center setup origin. Or, should I try to find another zero point which would be on the piece that is holding the box (which is a cylinder).

Thanks for your help! 

[Anonymous]

HI All, 

I'm new to Fusion and CAM in general and I've been trying to find how to setup my rig. 

Let me describe my setup:

I have a three axis CNC mill with a 4th axis aligned with the Y axis.

Mounted on the fourth axis, I have a box on which I need to machine four faces. Box rotates and Z goes down and holes are cut.

I got all that figured out but I have difficulty in getting a reliable location for zeroing my G54. I initially designed the CAM setup to have a WCS zero on a corner of the box but when checking the G code I realized that the heights were calculated that point and not from the individual faces that are defined in the tool orientation. That was a little unexpected since these menus show distances according to these face coordinate systems... but anyways...

I kind of have a working setup now where if I put the setup origin on the rotation axis I have all the limits heights OK but now, I would have to zero from the middle of the piece which is quite difficult, as least given my current knowledge of things. 

So my question is, what is the best way to go about that? Should I keep the setup zero on the rotation axis and find an external way to find my G54 zero. Or should I try to find a way to get the limits and heights right with Fusion with an off center setup origin. Or, should I try to find another zero point which would be on the piece that is holding the box (which is a cylinder).

Thanks for your help! 

[paul.clauss · Accepted solution]

Hi @Anonymous

Thanks for posting! As you have found, you must have the center of rotation for your rotary axis at the desired center of rotation (COR) for your part during machining - the rotary axis needs to be defined accurately just like the translational axes. In your case, this will require you to set up the part so that the rotational axis rotates around Y.

With this on-center setup, it can be difficult to approach zeroing the machine. However, because the COR is now in line with the center of the part, you could find the at the corner of the box using your current procedure and then simply jog the machine in Z and X to the center of the part - as defined by your WCS in Fusion. For example, if you find the top front corner of the stock, you will need to move the machine in X by (Stock Width/2) and in Z by (Stock Height/2). This is shown in the picture below:

After jogging the machine to the COR, you can set your G54. Because Y0 is easily found while initially finding the corner of the stock box at the machine, you will only need to jog the machine in X and Z.

Hopefully this helps! Please let me know if you have any questions.

[daniel_lyall]

Also have the origin pointing like it is in Paul's pick, It can be at the front or back of the stock

[Anonymous]

OK, I did try that but reviewing the G-code leaves me terrified...

with the g-code that I get from fusion, the spindle will crash every time I finish a face... Why is there that G28 G91 Z0, I mean, the simulation doesn't show that.

I don't mean to start a side discussion here but if I need to put my reference point at the center of the piece to get the limits right, the CNC shouldn't get the Z0 command...? Where's that coming from? Putting the zero in the middle of a solid surface seems like a recipe for disaster especially if random code gets generated from god knows where... Pretty steep learning curve here...

I'm popping a beer right now...

(CU_V5)
(BOX CUTTING)
(T1  D=3. CR=0. - FLAT END MILL)
G90 G94 G40 G49 G17
G21
G28 G91 Z0.
G90
(FRONT)
M9
T1 M6
S5000 M3
G54
G0 A0.
M8
G0 X0. Y-23.
G43 Z53.9 H1
Z26.7
G1 Z25. F1000.
X-0.044 Y-23.044
G17 G3 X0. Y-23.087 I0.044 J0.
Y-22.913 I0. J0.087
Y-23.087 I0. J-0.087
X0.044 Y-23.044 I0. J0.044
G1 X0. Y-23.
G0 Z31.95
X-0.3 Y-16.75
Z26.764
G1 Z25.064 F1000.
G19 G2 Y-17.05 Z24.764 J-0.3 K0.
G1 Y-17.2
G17 G3 X0. Y-17.5 I0.3 J0.
Y-12.5 I0. J2.5
Y-17.5 I0. J-2.5
X0.3 Y-17.2 I0. J0.3
G1 Y-17.05
G19 G3 Y-16.75 Z25.064 J0. K0.3
G0 Z53.9
G17
G28 G91 Z0.	
G90
(RIGHT)
G0 A90.
M8
G0 X0. Y-13.9
G43 Z53.95 H1
Z42.916
G1 Z41.216 F1000.
X-0.044 Y-13.944
G3 X0. Y-13.988 I0.044 J0.
Y-13.812 Z40.716 I0. J0.088
Y-13.988 Z40.216 I0. J-0.088
Y-13.812 Z39.716 I0. J0.088
X-0.063 Y-13.961 Z39.344 I0. J-0.088
X0.063 Y-13.839 I0.063 J0.061
X-0.063 Y-13.961 I-0.063 J-0.061
X-0.001 Y-13.962 I0.031 J0.03
G1 X0. Y-13.9
G0 Z53.95
G28 G91 Z0.
G90
(BACK)
A180.
M8
G0 X-25.168 Y-10.75
G43 Z54. H1
Z28.837
G1 Z27.137 F1000.
G19 G3 Y-10.45 Z26.837 J0.3 K0.
G1 Y-10.3
G17 G3 X-25.468 Y-10. I-0.3 J0.
Y-21.5 Z26.337 I0. J-5.75
Y-10. Z25.837 I0. J5.75
Y-21.5 Z25.337 I0. J-5.75
Y-10. Z24.837 I0. J5.75
X-29.647 Y-11.801 Z24.707 I0. J-5.75
X-21.288 Y-19.699 I4.18 J-3.949
X-29.647 Y-11.801 I-4.18 J3.949
X-29.635 Y-12.225 I0.218 J-0.206
G1 X-29.526 Y-12.328
X-29.478 Y-12.374 Z24.715
X-29.432 Y-12.418 Z24.737
X-29.39 Y-12.457 Z24.772
X-29.356 Y-12.489 Z24.82
X-29.33 Y-12.514 Z24.877
X-29.314 Y-12.529 Z24.94
X-29.308 Y-12.534 Z25.007
G0 Z54.
G28 G91 Z0.
G90
(LEFT)
A270.
M8
G0 X0. Y-13.9
G43 Z53.95 H1
Z42.916
G1 Z41.216 F1000.
X-0.044 Y-13.944
G3 X0. Y-13.988 I0.044 J0.
Y-13.812 Z40.716 I0. J0.088
Y-13.987 Z40.216 I0. J-0.088
Y-13.812 Z39.716 I0. J0.088
X-0.063 Y-13.961 Z39.344 I0. J-0.088
X0.063 Y-13.839 I0.063 J0.061
X-0.063 Y-13.961 I-0.063 J-0.061
X-0.001 Y-13.962 I0.031 J0.03
G1 X0. Y-13.9
G0 Z53.95
M9
G28 G91 Z0.
A0.
G28 X0. Y0.
M30

[innovatenate]

Hi There!

There was an issue and this post was delayed from being posted. We are looking into the issue. Sorry about that! It looks like you were able to get some help in the below forum post. 

https://forums.autodesk.com/t5/fusion-360-support/4th-axis-machining-heights-wcs/m-p/7166545#M4697

Hope all is going well!

Thanks,

[paul.clauss]

Hi @Anonymous

Thanks for the response! I think I can clear up the confusion around the G28 G91 Z0 line.

The G28 command prompts the tool to go to a position relative to machine home, not the work coordinate system home (as defined by the WCS setup in Fusion). The G91 line then turns the controls to incremental mode - meaning when the code on following the G91 will refer to the incremental distance from the previous position, in the case of your code Z53.9.  Because of this, the Z0 in your code is basically meaningless, as the incremental Z-distance from the previous position is zero (during the G28 move to machine home). 

G19 G3 Y-16.75 Z25.064 J0. K0.3
G0 Z53.9
G17
G28 G91 Z0.

 The first line will select the YZ plane for arcs (G19) and lead out of the cut. The machine will then rapid (G0) to Z53.9 (based on the part/work coordinate system). The G17 sets the arc plane to default (XY) and then the G28 G91 tells the machine to go to a point relative to machine home, at Z0 from the previous position. I would expect the code to make the machine arc out of the cut, retract straight up to Z53.9, and then retract directly to machine home - usually near the tool change location for most machines/controls.

The caveat here is that your machine coordinate system can not be at the same location as your work coordinate system (defined in the Fusion setup). I also believe that Fanuc controls may act a little differently - I am unsure of what machine and controller you are working with. I would recommend doing a dry run (with no stock in the machine) of your code - you will be able to see if there is anything unique going on that causes the tool to move to the WCS easily.

Please be careful testing at the machine and let me know if anything is not working as intended! I look forward to hearing the results.

[daniel_lyall]

Before this goes any where further @Anonymous what is your machine controller.

The A axis moves are done at G28 so your Z is right out of the way, In the pre post dialog you can turn G28 off and use G54 whats G53 + 1 or the first off set you set, by homing the machine.

[Anonymous]

It's a Cnc3040t with TX14207 drivers. I'm running this with Mach3

I'll have to read that post a couple of times and do some research to build some knowledge base on my side.

I really appreciate your help, I will follow up as soon as I have something intelligent to say. Regards.

[daniel_lyall]

I tested your code in Mach3.

Do you know how to home the machine and set the work zero (not homing the machine will more than likely destroy your spindle and 4th axis) this is an important question

[Anonymous]

I do know how to home the machine.

As a precision, I never ran this code live on the machine only in Mach3 as precautionary measure.

I suspect that I did not do the homing procedure correctly in the offline mode which led to the machine coordinates and the G54 to overlap.

Somehow it didn't sound obvious that if I would set a clearance height there would be an additional command added to clear the bit away from the jig. There certainly is a good reason for this that I'm not aware of but seems like a lot of time spent jogging around.

Thanks for all your help, you guys really are awesome

[daniel_lyall]

---

@Anonymous wrote:
I do know how to home the machine.

As a precision, I never ran this code live on the machine only in Mach3 as precautionary measure.

I suspect that I did not do the homing procedure correctly in the offline mode which led to the machine coordinates and the G54 to overlap. that will be it

Somehow it didn't sound obvious that if I would set a clearance height there would be an additional command added to clear the bit away from the jig. There certainly is a good reason for this that I'm not aware of but seems like a lot of time spent jogging around.

Thanks for all your help, you guys really are awesome

---

Clearances hight is your safe to move hight 

[michel.lebois]

please I can not configure fusion for the rotary 4 axis in y you can help me not as well as doing post processing, do you have one?

[daniel_lyall]

@michel.lebois can you start a new post things are different now.