Reply with QuoteSample of G-Code & Where you are having trouble?
G41 HAAS TL1 lathe problem
Hello all!
I want to know what is the correct way in order to program an ID G41 lathe program.
I'm having problems with the radius because they appear upsidedown.
My machine is a Haas TL1 Year: 2004
Thanks for your help.
Best regards.
Re: G41 HAAS TL1 lathe problem
Sample of G-Code & Where you are having trouble?
(I am using mm.)Originally Posted by SumDumPhuckr
I am using a 0.4 radius tool tip 2
Please check the images attached.
G Code:
o00135;
T808 M08;
G97 S1000 M03;
G55 G00 X18. Z2. F0.2;
G50 S1000;
G96 S180;
G41 G00 X19.;
G01 Z1.;
G71 P3 Q4 D0.2 U-0.1 W0. F0.2;
N3 G01 X22.2 Z0.;
G02 X21.8 Z-0.2 R0.2;
G01 Z-0.66;
G02 X21.81 Z-0.69 R0.2;
G01 X22.39 Z-2.46;
G03 X22.33 Z-2.7 R0.41;
G01 X20.591 Z-4.656;
G01 Z-5.456;
N4 G00 X19.791;
G70 P3 Q4 F0.1;
G40 G00 X17.;
G97 S700;
M05;
M30;
Thank you.
Attachment 277647
Attachment 277649
Attachment 277651
Re: G41 HAAS TL1 lathe problem
Try this program.
o00135;
T808 M08;
G97 S1000 M03;
G55 G00 X18. Z2. F0.2;
G50 S1000;
G96 S180;
G00 X19.;
G01 Z1.;
G71 P3 Q4 D0.2 U-0.1 W0. F0.2;
N3 G01 X22.2 Z1.
G41 Z0.;
G02 X21.8 Z-0.2 R0.2;
G01 Z-0.66;
G02 X21.81 Z-0.69 R0.2;
G01 X22.39 Z-2.46;
G03 X22.33 Z-2.7 R0.41;
G01 X20.591 Z-4.656;
G01 Z-5.456;
G01 X19.;
N4 G40 G1 X17.;
G70 P3 Q4 F0.1;
G97 S700;
M05;
M30;
Re: G41 HAAS TL1 lathe problem
Image processing on the modified program.
Attachment 277914
Dear andre_77 I couldnt see the attachment.
I'm gonna test your code and will let you know about it
Thank you
Re: G41 HAAS TL1 lathe problem
Dear Andre,
I did the test with the code you suggested but it gives an "code R error"
Im attaching a tool picture. DCGT 070204
What else can I do?
Thank you.
PS: What is that software you are using? What did you use in order to record the video???
Re: G41 HAAS TL1 lathe problem
I'll try to check the program at work. I use a program CAMplus KELLER see more here cnc-keller.com.
Very good! What did you use for recording the video?
Thank you
Re: G41 HAAS TL1 lathe problem
G71 cycle when using the G41 can not process your circuit if the tool nose radius more than 0.2 mm. Finishing without cycle but using command G41 and tool nose radius 0.4 mm possible.
I suggest you try the next version of the program. Roughing without the G41, but given the range by changing the coordinates of the contour points. Finishing with G41 (radius 0.4 mm).
For video recording, try searching HyCam
O00138
(r0.4)
T808 M08
G97 S1000 M03
G55 G00 X18. Z2. F0.2
G50 S1000
G96 S180
G00 X19.
G01 Z1.
G71 P3 Q4 D0.2 U-0.1 W0. F0.2
N3 G00 X23. Z1. M08
G01 Z0. F0.15
G02 X21.8 Z-0.6 R0.6
G01 Z-1.06
G02 X21.803 Z-1.096 R0.4
X21.824 Z-1.166 R0.6
G01 X22.401 Z-2.925
G02 X22.402 Z-2.93 R0.4
G03 X22.401 Z-2.936 R0.01
G02 X22.399 Z-2.938 R0.4
G01 X20.66 Z-4.894
G02 X20.591 Z-5.056 R0.4
G01 Z-5.456
N4 X18.
G01 X22.2 Z1.
G41 Z0.
G02 X21.8 Z-0.2 R0.2
G01 Z-0.66
G02 X21.81 Z-0.69 R0.2
G01 X22.39 Z-2.46
G03 X22.33 Z-2.7 R0.41
G01 X20.591 Z-4.656
G01 Z-5.456
G01 X19.
G40 G1 X17.
G00 Z1.
G97 S700
M05
M30
Dear Andre it worked with your suggestions! Thank you very much!
The code is in the attachments
Re: G41 HAAS TL1 lathe problem
Please, I wish you good luck in the work.
Why are you working with such a small depth of cut?
Your preform has high hardness?
In my opinion your cutter is not really suitable for such treatment may be better to use a tool similar to the tool in the video.
Posting Permissions
