Having trouble with touch off

Hello Folks

Thanks for the comments,

I will try them out next week and get back to you. My wife and I are off camping this weekend and I won't get a chance to play around with the mill until next Tuesday.

Chipmunk

Hello Folks:

I started from scratch and reset up my mill using the comments and suggestions from you people. Needless to say, I found and corrected a number of problems.

First of all I determined what my limits and travel is for each of the axis's and set the limits accordingly in the configuration for my mill. I decided that the bottom left hand corner will be my zero for the X and Y limits and the top of the column will be the 0 for the Z limit. The X travel is 0 to 11.625, the Y travel is 0 to 4.875 and the Z travel is 0 to -5.75. I then jogged all of the axis's to some value that moved them off of the home position and invoked G53 G0 X0 Y0 Z0 , the mill responded correctly.

I then set my G54 tool off set using a 0.0015 feeler gauge. Using the left hand side of the work I set the X offset to -0.0015 the Y offset was set at the bottom of the left hand side to -0.0015 and the Z offset was set to +0.0015 off of the to of the work piece. I then invoked G53 again and all off the axi's went to the home position.

I then edited the program and added G54 to the preamble.

The next move was open up the work program and home all of the axis's , they were already at zero because of the previous G53 command. I started the program and was immediately met with a error message, (Program Exceeds Maximum on the Z Axis) I pushed run anyway,

I then was greeted with another error message (Linear move on line 5 would exceed joint's positive limit.)

That is where I am at now, attached is the the first 24 lines of my Cut 2 D program.

%
G20 G40 G49 G54 M6 T1
G17
M7
G0Z0 0.7874
G0X0.0000Y0.0000S7000M3
G0X-0.0938Y0.5159Z0.2362
G1Z-0.0625F0.5
G1Y1.0309F3.0
G2X0.0000Y1.1247I0.0938J0.0000
G1X0.7976
G1X0.8354
G1X0.8420Y1.1247
G1X0.8491Y1.1247
G1X0.8565Y1.1247
G1X0.8643Y1.1248
G1X0.8725Y1.1250
G1X0.8809Y1.1252
G1X0.8895Y1.1255
G1X0.8983Y1.1259
G1X0.9073Y1.1264
G1X0.9163Y1.1271
G1X0.9253Y1.1278
G1X0.9342Y1.1288
G1X0.9430Y1.1298
G1X0.9516Y1.1310
G1X0.9600Y1.1324
G1X0.9680Y1.1339
G1X0.9756Y1.1355

Could you please have a look at this and advise me as to what to do.

Thanks Chipmunk

which post processor are you using with cut2d ?
and after homing are you setting the z axis to the top surface of the work and setting to work z0 touch off etc ?
if not then that is the reason for the exceeds limits error

OK, the move exceeds limit mans the machine is not properly set up. Do you have home switches?
If not, you really should set up one of the methods of homing the machine to limit switches.
Once you have the machine homing to a repeatable position, then move the machine to
the limits of mechanical travel and observe the coordinates in the machine coordinate system
(G53 or I think pressing the @ will display that coord system.) You will apparently have to
expand the limits in the .ini file where you have MIN_LIMIT and MAX_LIMIT in the axis
that is hitting the limit (Z is the first one, but you may have others when you clear this one
up.) Once you know the limits of travel, then use these values in the .ini file for
MIN_LIMIT and MAX_LIMIT. Then, as long as your workpiece and program fit in
these limits, you should not get these messages anymore. The great thing about
setting all this up is that when you load a part, touch off and then load the program,
you will get a message if the program would exceed the limits before you even hit run!
You then can reposition the part before starting so there will be no problem.

Jon

Hello

cnbasher I am using EMC2 Arcs (inch) * ngc for my post processor.

Jmelson You are correct in saying that my move is outside my machine coordinates. It was not the setup of the machine it was a bad entry in the Cut2D material size. I inadvertently put in a to large value in G0Z0 .7854 this value was outside of the box and gave me the error message. I reduced this value to .125 and the program started running quite happily. The reason I did not have a problem when I was cutting air was because I did not do a touch off from my vise which is about 4 inches above the table. Given that I only have 5.75 inches of Z travel, it made my upper limit very close to the top of the work area box. I need to purchase a vise that does not take up as much room.

BigJohnT Also I did not take into consideration half the diameter of my tool bit when setting my touch off. I re read the article on touching off, it is surprising how much comes to light during subsequent readings.

In summary I made my first part this evening and it worked out very well. Thank You Folks for all of your help without it I would still be struggling.

From a Happy Chipmunk who finally made some chips.