Probing issue with rectangular block- trying to cut the first part but Y axis lifting after fast touch-off

[Elemental_Garage]

Hey all,

Got my machine setup and ready to cut my first part. Nothing fancy, just cleaning up a scrap block to turn into a little candle holder for the GF.

When running the probing routing for the rectangular block is touches off the X just fine, but when doing the Y it will do the fast touch, then lift the -.5" I set for the Z offset to do the slow touch, and then error out. As I'm new I fully expect this is a user error, but just thought I'd ask here in case this is a macro issue or something else.

Here is a video: https://photos.app.goo.gl/p8u5vtVeN3768ruk6

Thanks all!

 

[Elemental_Garage]

I tried to be clever and use a Web-X and then Web-Y separately, but the rectangle block likely just calls on those and combines them, as the Web-Y does the same thing as in the block mode.

 

[PriddyShiddy]

Almost definitely the Y value is too large, or you have it positioned too far off Y center. It is triggering before or after the expected position which sends 'Probe Fail'. Does it all the time when I center on large plates and am .375" off center. I just jog a little the other way and check the dimension I put in.

 

[Elemental_Garage]

You might be right. I took it from 2.5 down to 2.4 and it completed the probe job. I guess it's more picky than approx tool length values.

 

[GiroDyno]

Are you probing using the control? Or CAM?
Can be really annoying how tight the default under/over travel values are using the controller probing cycles. I assume it just uses Renishaws 3mm by default which can be hard to eyeball particularly on larger travel machines and parts in the back corners of the table. If I knew where the damn part was I wouldn't need to probe it!

 

[Elemental_Garage]

Probing via the control. Yes, the instructions say to input a size greater than the part, so I was just playing it safe I guess, and oversizing it too much.

I see you're in the PNW as well! Hello from the Portland'ish area.

 

[GiroDyno]

Renishaws default tolerance for over/under travel is 3mm ~1/8" so you need to enter values that combine the error of your starting position (relative to center) and the size of your part that add up to less than 1/8"
You can say your part is 2.5 when its really 2.4, but then you need to also start ~ .025" from center or its going to exceed that 1/8" tolerance band.
There's also no reason not to enter the actual size if you know it, then all of your tolerance band can be dedicated to how well you centered the probe over your part.

I generally stick with single-axis cycles when probing on the controller because I can much more easily eyeball being 1/2" away from the part (+/- 1/8") than can eyeball being I within 1/16" of center and entering the size within 1/16" as well. Once you recognize the code it generates in MDI you can adjust the values there and switch between axis and dimensions from the first single-axis cycle it spit out faster than going back into VPS or whatever its called and making a new routine for each axis.

And hello from Bellingham!

 

[Elemental_Garage]

That's good to know. To overcome my issue last night I just did a single side measurement, recorded the machine position, and then did the opposite side, halved the distance and jogged the machine to that half, and made that my Y G54. Glad we figured out the issue (user error in this case) so that I don't have to do that each time haha.

 

[rjwalker1973]

You can also override the default travel tolerance with a Q value. If for instance you wanted to use .500 instead of .375 as is the default.
EX.
G65 P9812 X2.5 Z-.35 S1. Q.5
G65 P9812 Y2.5 Z-.35 S1. Q.5
This will override the default tolerance for this probing cycle and use .500 instead of .375