Postprocessor modification 4 axis

[DominikRek]

Hi, can anybody help me with modify postprocessor for 4 axis machine please??

it is yilmaz 4410 with ISO control.

 There is reversed Y axis, G2 and G3 is reversed and head A axis around X do not support TCP.

5axismaker post is working fine after reversing Y G2 and G3 but have problem with fourth axis.

Thanks

[DominikRek]

---

[andrea.amilo]

Hello @DominikRek ,

 
I understand that you have already modified the 5axismaker post to suit your needs in 3 axis.
Are you able to work correctly in 3 axis?
if so, you should select a 4 axis machine in the library or create your own to match your postprocessor.

Here are some links to the Fusion machine documentation that may help you:

Fusion Help | Workflow: Using and creating machine definitions | Autodesk
Fusion Help | The Machine Library | Autodesk

Please let me know.
Thanks. 

[DominikRek]

yes already modified it and works good for 3 axis operations, tried configure machine but do not work properly for 4 axis machining. I do something wrong

[DominikRek]

With machine configuration pivot length and tool length aren't added to Y and Z values

[andrea.amilo]

Hello @DominikRek,

I believe you con define the pivot length in the 'advanced settings - offset' field (as shown below) with the TCP option off:

Once this is done, the tool length defined in Fusion should be properly considered in your nc-code.

Please test it very carefully and let me know.

Thanks.

[DominikRek]

Thanks for that. Now when try to machine only 3 axis post is adding tool and pivot length even if head is at 0 degree position so my top surface is Z+ tool length + pivot length.

(2D CONTOUR1)
M5
T2 M6
S8000 M3
G17 G90 G94
G55
G0 A0.
G0 G43 X1061.42 Y31.227 Z313.61 H2
G0 Z258.61
G1 Z254.61 F1500.
X1061.06 Y31.052 F1440.
G2 X1061.802 Y33.19 Z254.39 R1.6 F1500.
X1063.94 Y32.448 Z254.17 R1.6
 

A-90 is fine

(2D CONTOUR1 2)
G0 A-90.
G0 G43 X1024.42 Y377.11 Z-56.227 H2
G0 Y322.11
G1 Y318.11 F1500.
X1024.06 Z-56.052 F1440.
G18 G3 X1024.802 Y317.89 Z-58.19 R1.6 F1500.
X1026.94 Y317.67 Z-57.448 R1.6
X1026.198 Y317.45 Z-55.31 R1.6
X1024.06 Y317.23 Z-56.052 R1.6
X1024.802 Y317.011 Z-58.19 R1.6

[DominikRek]

anybody can help me solve this problem please?

[andrea.amilo]

Hello @DominikRek ,

I have noticed in your example nc-code that you are using the toollength compensation function (=G43):

Since your postprocessor now recalculates the distance from the tool tip to the machine pivot point, I assume you don't need to use G43.

Otherwise, in a 3 axis program, the distance will be calculated twice.

Please try not to use G43:

Please test it with great care and attention and let me know.

Thanks.

[DominikRek]

Yes, but this isn't my problem. The problem is that when the head is vertical, fusion should generate a program without adding any values ​​to Z. If Z is set at the top and the head is vertical, the program should generate code as for a normal 3-axis machine. Only after I rotate the head by a given angle should the calculations of new coordinates begin so that the tool tip is where it should be. The problem is that these calculations are incorrect because despite various modifications to the settings, I am not able to achieve the correct coordinates in the Z and Y axes. I only manage to set one of the axes correctly, then the other is wrong or vice versa. For example, when I rotate the head by 90 degrees, the Z axis should be lowered only by the length of the pivot and the Y axis should be moved away from the processed element by the length of the pivot and the length of the tool, despite trying to change the settings, the Z axis is also lowered by the length of the pivot and the length of the tool, and in this situation the tool length should not be added to the Z coordinates

[DominikRek]

[andrea.amilo]

Hello @DominikRek ,

I did a simple test using the suggested configuration.

I hope this could help you to understand how the post calculation works for non-tcp heads.

I have milled a box using a trace toolpath:

The trace was on a face 25 mm distance from the origin + 150 mm of TCP distance + 90.34 mm toollength.

So:

              Y = 25 + 150 + 90.34 = 265.34

              Z = 0  = approach at the top of the box

This is what I achieved:

I would say the output is as expected.

Can you please tell me what doesn't work in this example for you?

Please let me know.

Thanks.

[DominikRek]

Thank you for that. I use different machine and it is looking better now 

(1001)
(T1 D=2. CR=1. - BALL END MILL)
G21
G40
G49
G80
G90
G28 G91 Z0.
G90
G0 A0.

(TRACE1)
M5
T1 M6
S8000 M3
G17 G90 G94
G54
G0 A0.
G0 X25. Y25. Z216.
G0 Z205.
G1 Z200. F750.
X-25. F1280.
Z205.
G0 Z216.
G28 G91 Z0.
G90

(TRACE1 2)
G0 A-90.
G0 X-25. Y241. Z0.
G0 Y230.
G1 Y225. F750.
X25. F1280.
Y230.
G0 Y241.

G28 G91 Z0.
G90
G0 A0.
G28 G91 X0. Y0.
G90
M0
M30

So with this configuration when I setting Z0 I have to consider pivot length. Actual part Z0 will be set to 4th axis rotation point not to spindle face. Am I right?

[andrea.amilo]

Hello @DominikRek ,

I would say don't use the G43 function, as you did.

Having said that, I don't know if this is enough for your controller to not take into account the tool length or if you are forced to define the zero point on the pivot.

I would suggest that you contact the machine support (if possible) or test it very carefully on your machine.

Thanks.

[DominikRek]

however it is wrong, after rotating the head 90 degrees Z should be lowered by the length of the pivot, because the head is as if shortened by this length if you know what I mean

[DominikRek]

No sorry if Z0 will be in centre of rotation that is good

[DominikRek]

Thank you, rotation is working fine now.

Got another problem. Noticed that bores are not perfectly round, checked machine parameters and machine arc tolerance is 1mm. Can I change it in post processor to generate less lines when milling bores?

[andrea.amilo]

Hello @DominikRek,

I am happy to learn that now the rotation head on your machine seems to work well.
If so, please click on the "Accept Solution" tab: it could help other Fusion users with the same machine kinematics.

Thanks

[andrea.amilo · Accepted solution]

Hello @DominikRek ,

the following code lines handle the arc configuration in your postprocessor:

This is a Post Processor Training Guide draft that explains the meaning of the circular parameters: 

If you wish, you could disable all circular interpolation by setting the allowedCircularPlanes to 0.

I hope this could help you.

Thanks.

[DominikRek]

Thank you for help.

Positioning before milling is done in 3 axes simultaneously and sometimes it can cause collisions. How can I change it and select which axis want to move first?