1. GCode and Part Programs
  3. G&M Codes
  5. Problem with G41/G42 command

Problem with G41/G42 command

More
05 Nov 2011 11:14 #14590 by pklecz
Problem with G41/G42 command was created by pklecz
I have got a problem because Emc2 dont want to compensate.

G21
G90
G64 P0.01
G17
G40
G49
G10 L1 T1 R1.17
T1M6
M8
S5000M03
G0 Z 15.000
G0 X 53.077 Y -5.541
G0 Z 3.000
F150
G1 Z -0.500
F400
G41 D1
G1 X 54.247 Y -3.041
G3 X 50.577 Y 0.629 I -3.670 J 0.000
G1 X 0.577 Y 0.629
G1 X 0.577 Y 50.629
G1 X 50.577 Y 50.629
G1 X 50.577 Y 0.629
F150
G1 Z -1.000
F400
G1 X 0.577 Y 0.629
G1 X 0.577 Y 50.629
G1 X 50.577 Y 50.629
G1 X 50.577 Y 0.629
G1 Z 3.000
G0 Z 15.000
G40
G0 X 0.000 Y 0.000
M9
M5
M2

Pliz help me this is a simple square and Emc2 dont want to compensate the tool diameter.

Please Log in or Create an account to join the conversation.

More
05 Nov 2011 22:02 #14597 by andypugh
Replied by andypugh on topic Re:Problem with G41/G42 command
You forgot the G43.

T1 M6 loads tool 1, but you need a G43 to apply the tool offsets.

Please Log in or Create an account to join the conversation.

More
06 Nov 2011 18:21 #14613 by pklecz
Replied by pklecz on topic Re:Problem with G41/G42 command
I tried with g43 but it do not work.

I think i tried everything. I even tried to reinstal the system but it do not work.

Maybe if you could send me a simple gcode of a square 50x50 mm that works for you with a tool compensation.

Iam desperative now i dont know what iam doing wrong :(

Pliz help

And thx for help

Please Log in or Create an account to join the conversation.

More
06 Nov 2011 20:27 - 06 Nov 2011 20:47 #14615 by BigJohnT
Replied by BigJohnT on topic Re:Problem with G41/G42 command
Did you look at the examples in the manual?

After adding G43 to your tool line what didn't work? You need to be specific to get help. Does the tool table contain the proper diameter of the tool loaded?

I loaded your code and added G43 but I get an error on line 7 about your G10 P value being out of range.

When I comment the G10 line I get an error about lead in move too small for tool diameter but I don't know what diameter your using.

And there is no T word for G10 L1...

Fixing the G10 error I'm back to you didn't program a long enough lead in move...

Fixing the lead in move and you have moves that are too big for the tool diameter...

Switching to inside the box compensation G42 your file runs with the G10 line fixed as well...

John
Last edit: 06 Nov 2011 20:47 by BigJohnT.

Please Log in or Create an account to join the conversation.

More
06 Nov 2011 20:48 #14616 by pklecz
Replied by pklecz on topic Re:Problem with G41/G42 command
Yes I did look at the examples in the manual.

When I add G43 to my gcode there is no tool compensation when I run the gcode.

Iam using a tool 2.34 [mm] wide. The radius of my tool is 1.17 [mm].





PS: I had no problem with tool compensation earlier, but then one day The EMC2 stoped to compensate the tool diameter. I had runed the same gcode as earlier but it didint work. I even had reinstaled the whole ubuntu with emc2 but this didint work. So maybe it is something with the Emc2 i dont know.


Thx for all reply

Please Log in or Create an account to join the conversation.

More
06 Nov 2011 20:59 #14617 by BigJohnT
Replied by BigJohnT on topic Re:Problem with G41/G42 command
Did you fix the G10 L1 line?

John

Please Log in or Create an account to join the conversation.

More
06 Nov 2011 21:58 #14619 by pklecz
Replied by pklecz on topic Re:Problem with G41/G42 command
Now I have corrected the g10 line and it works. Thank you werry much :)

Now I will write how i solve my problem

So

G10 L1 P1 R1.17 (This line sets in the Tool Table in the first position in the tool table (L1) in the first pocket (P1) tool with the radius of 1.17).
G43 H1 (This command activates the tool table and it is important to show what kind of tool will you use in this case H1 where 1 is the first tool from the tool table)
And then
G41 or G42 after the lead move.


PS: My first problem was in the G10 command i wrote T1 and my Emc2 didnt show me an error. And my second problem was that I didnt write G43 with the H1. I write only g43 because iam stupid :P

Thanks all for your help

PS2: sorry for my english :P

Please Log in or Create an account to join the conversation.

  1. GCode and Part Programs
  3. G&M Codes
  5. Problem with G41/G42 command
Time to create page: 0.126 seconds
Powered by Kunena Forum