5-axis post help

[DavidB]

I want to put tilted work planes into my Generic Fanuc 5-axis post for 3+2 programming.

G68.2 X,Y,Z,I,J,K

 

Also G43.4 for 4 and 5-axis simultanous toolpaths.

 

 

Thanks Dave

[Josh T™]

That's gonna be a lot of work Dave. Something like this is gonna be WAY beyond my skills.

 

Good Luck!

[HT]

Dave, i maybe wrong. Your machine is table-table i don't think you need G68.2 at all, if you program tool tip you need G43 for positioning like a horizontal and turn on G43.4 for 4 and 5-axis simultanous toolpaths.

[DavidB]

From what I can understand G43.4 turns ON TPC which I need for 5-axis simultanous toolpaths.

 

So can I just get the post to out put a G43.4 for 5-axis toolpaths?

 

The G68.2 I need for 3+2 toolpaths this is so I can put the work piece WCS anywhere on the table.

 

This is the first machine we have purchased a machine with TPC so my other 5-axis machines the post takes care of rotary positions. But the part must be in the same spot on the rotary as my CAD modal.

 

 

Thanks Dave

[DavidB]

How do I get the G68 tilt work plane to turn on and the G69 cancel function.

 

I can see that its in the post but what triggers it?

Is it Mi6

[HT]

Dave, try this:

#Output formatting

top_map : 1 #Output toolplane toolpaths mapped to top view

[DavidB]

Yeh I got that thanks. I have the post working correct except for TPC toolpaths so hopefully In-house can supply me with a post.

 

Cheers Dave

[HT]

[gcode]

TPC = toolpoint compensation ????

 

Have you tried changing

shift_z_pvt : 0 to 2

 

make sure

use_tlength = 0

toollength = 0

[Jimmy Wakeford from Barefoot CNC]

The inhouse post will take care of the tcp and also it will allow for the look ahead function settings (G05's). Look at the code carefully as it may invoke a g49 when using a G05. Depending on how your machine is setup this could be bad news.

 

When invoking tcp you want to be at a0c0.

To switch between G43 and G43.4 you can use a misc switch or check toolpathtype to determine which one. Then in the tool changes sections just set up two G43 output lines with if statements.

[DavidB]

Still no contact from In-house so patiently waiting.

 

Gcode my bad that should have been (TCP) Tool Centre Point control turned on by G43.4.

This means I can set the Work origin anywhere on the table

 

This is only for 5-axis toolpaths.

code:

---

( 5-AXIS SWARF )

M13

M11

T42

M6

H1 D2

M56

G0 G54 G90 X28.912 Y2.976 C0. B0. S14000 M3

T43

G43.4 H1 Z57.515

C-90. B-28.565

M8

---

For 3+2 it uses G68.2 (TWP) Tilted Work Plane command

 

code:

---

 ( POCKET C180. B-90. FRONT T/C PLANE)

Z400.

G49

X9.542 Y1.834

G68.2 X0 Y0 Z0 I180. J-90. K0.

G53.1

M12

M10

G43 H1 Z35.

---

[Watcher]

TCP

 

Good thing about it: The control handles everything so you only have to output the X/Y/Z/I/J/K values just like they are in the NCI

 

So for simultaneous moves you have to set the multaxis post-block (I don´t remember its name anymore... 4 years working with Pro/NC) to output a the G43.4 string before the multiaxis moves... the rest is G1 X/Y/Z/I/J/K values just like they are in the NCI

 

You will have to output G68.2 X,Y,Z,I,J,K from the NCI matrices for every operation but in this case the coordinates need to be mapped to the plane where the matrix is set...

 

This is were I would start...

 

Good luck!

[DavidB]

quote:

---

Have you tried changing

shift_z_pvt : 0 to 2

 

make sure

use_tlength = 0

toollength = 0

---

Thanks Gcode I tried but no differance.