5 Axis Post/CAM Issue

[Anonymous]

Hey Guys,

So Im trying to run a test piece on our Haas VF6 with a TR310 Trunnion.  My issue is when I post and run the program, my tool paths seems to be 180 deg out on the Z Axis.  Maybe my program is setup wrong, or something in my post file, Im not exactly sure.  Here is what I have so far:

SetupTool Path for "6 Side"

So after I post and run the program on my machine.... My first 4 toolpaths work out perfect since they are only running 3 axis, but when I go to run the 5 axis portion here is what I end up getting as a result...

%
O01001 (Die Test)
(Using high feed G1 F500. instead of G0.)
(T1 D=3. CR=0. - face mill)
(T2 D=0.5 CR=0.25 - ball end mill)
(T7 D=0.375 CR=0. - flat end mill)
G90 G94 G17
G20
G53 G0 Z0.

(6 Side)
T7 M6
(.375" Cutter)
S8000 M3
G54
M11
M13
G0 A90. C-180. (C-Axis should be 0.)
M10
M12
G254
M8
G0 X-0.545 Y-0.5 (This should be X0.545 Y0.5)
G43 Z1.6 H7
T1
G0 Z1.2
Z1.132
G1 Z0.875 F1.019
X-0.5435 Y-0.4999 F300.

What am I missing here? Is it my post or is it my setup? I have DWO/TCPC on my Haas.  The post Im using is the current Haas NGC post.  Seems like no matter what I do, my tool path starts 180 deg off. Is my G254/255 in the wrong spot? If I turn on G234 I get an error in my machine. Hopefully everything I said makes sense. I have attached my .f3d file as well.

Thank you for the help!

Jim

[Anonymous · Accepted solution]

I think whats going on here is your a axis is actually incorrect. Either your machine was setup incorrectly or you actually need a-90. c0 which is the other possible rotary solution. 

as far as the x and y axis they are relative to where the offset has moved to. The position stays the same but the z axis will "appear" to be wrong depending on what your looking for. Just trust the computer as 99.99 of the time it is correct.

tcpc is only active for simultaneous 5 axis movement and cannot be used in conjunction with dwo. 

I edited a post for the ngc and you just have to activate a axis and c axis when you go to post process.

Also from my knowledge and experience  with the ngc control, there cannot be an active a axis offset on the desired work offset to achieve the proper calculation. A axis has to be 0. C axis can have any value.

if you need any additional help trouble shooting this, send me an email and we can setup a call to resolve this issue. 

[email protected]

[Anonymous]

Thanks a lot for the help Devonm.dupius! You are right, it was my machine setup in my post processor.  Your post worked, I just had to switch it around so that the A-90 would be a positive value for me so that the trunnion was facing me instead of away from me. 

I still have one issue but I think it is with the DWO/TCPC instead but I need to run a few test samples to make sure.

[Anonymous]

OK let me know if you need help. 

no worries.

-D-

[Anonymous]

I am having similar issues but this fixed the x location. My Y is off, the tool is too far in front or + of the actual workpiece cutting air. The Z is also off and wants to go wayy to deep. Any advice?