3 Corner and UGS Problem

New to using UGS and Charley’s Triquetra 3 Corner finder and am coming up with an error when ever i try and run the gcode. If any one can point me in the right direction it would be much appreciated . It starts with this one then goes on with about 30 other errors.

What does your Gcode look like you’re trying to run?

This what the tool box gave me with my measurements.

G20
G92 X0
G92 Y0
G92 Z0
G38.2 X-0.5F2
G92 X1.99225
G91 G0 X0.5
G91 G0 Y1
G91 G0 X-1
G38.2 Y-1 F2
G92 Y2.09825
G91 G0 Y0.125
G91 G0 Z1.019
G91 G0 Y-0.625
G38.2 Z-1 F3
G91 G0 Z0.05
G38.2 Z-0.2 F1
G92 Z0.8140
G91 G0 Z0.125
G91 G0 X1
G91 G0 Y1

Ok it ended up being the version of UGS i was using, but now it only does x and y and skips the z part

You’re issuing two probing commands for the Z axis. Why?

Your last 7 lines are these:
G38.2 Z-1 F3
G91 G0 Z0.05
G38.2 Z-0.2 F1
G92 Z0.8140
G91 G0 Z0.125
G91 G0 X1
G91 G0 Y1

Replace them with these and try it.
G38.2 Z-1 F5
G92 Z0.8140
G91 G0 Z0.125
G91 G0 Y1 X1

ok iwill try that, this is what UGS is telling me when it skips

G38.2Z-‪5.08‬F25.4
ok

G92Z8.1200
error: Bad number format

G91G0Z3.175
G91G0x25.4
error: Bad number format

G91G0Y25.4

error: Bad number format
error: Bad number format
error: Bad number format
ok
ok
ok
ok

just tried that code you gave, it made a different sound like it wanted to do something but then stopped

ok

G91G0Y1X1
[PRB:-524.737,-654.912,-17.822:1]
ok
ok
ok
error: Bad number format
error: Bad number format
ALARM: Probe fail
[PRB:-524.737,-654.912,-17.822:0]
ok
error: Alarm lock
error: Alarm lock

@CharleyThomas any ideas what I am doing wrong?

Here’s my script:

G92 X0
G92 Y0
G92 Z0
G20
G38.2 X-0.5F5
G92 X2.0175
G91 G0 X0.5
G91 G0 Y1
G91 G0 X-1
G38.2 Y-1 F5
G92 Y2.0605
G91 G0 Y0.125
G91 G0 Z0.9
G91 G0 Y -0.625
G38.2 Z-1 F5
G92 Z0.8214
G91 G0 Z0.125
G91 G0 Y1 X1

On the G92 lines immediately following the 38.2 lines, change the values I have for measures of my touch plate and use yours. Clear your errors with a ‘$X’ to clear that alarm lock first.

That worked, thank you so much

Glad to help!

Sorry for not getting on this sooner. I have been in the shop all day. So are you good now?

By the way, the reason for probing the Z axis twice is to insure the most accurate zero as possible. I had experienced some problems if the z axis is probed at too high a feed rate so I added the second probe at 1 inch per minute.

No, i used Traxxtar’s gcode he provided me with changing my dimensions, but anytime i use the tool box it gives me an error

1 Like

I was also receiving the same error (bad number format with garbled output), but used the code posted above by Traxxtar to fix my issue as well. Thanks!

1 Like

So I figured it out, all I had to do was delete and move the G20 below the G92 Z0

G20 simply insures that you are operating in inch mode. G21 would change it to mm mode. If you manually change the code to match the measurements of your particular touch plate be sure to add the radius of your bit to that measurement or the location of your zero will be off by that amount.

This is done on the G92 X .__ and the G92 Y .__ lines of the code where:

Example: If you have a touch plate that measures 2.100 inches in X and 2.200 in Y and you are zeroing with a 0.25 inch bit then:

  G92 X _.___ = Touch Plate X axis measurement + Bit Radius (1/2 bit diameter)
              G92 X 2.225   (2.100 + 0.125 = 2.225)
  G92 Y _.___ = Touch Plate Y axis measurement + Bit Radius (1/2 bit diameter)
              G92 Y 2.325   (2.200 + 0.125 = 2.325)
1 Like

If anyone else is having this issue please let me know. I have made a change to the Triquetra Tool Box that I believe will resolve the issue. Before I publish the update I need to find someone else who is having this issue and I will send you a link to download the fix. If that works then I will publish it for everyone as an update to the Triquetra Tool Box.

Charley Thomas
Triquetra CNC