Need help with Renishaw probing - Haas machine

Hey guys, hoping someone can help me out with a probing question. I seem to remember on an older Haas machine I ran (2010?) that on the edge find routines for the probe cycle they had a shift value you could put in. Anyone else remember that? Now I know I could pick up the edge and then manually type in +.01 or whatever, but I want the machine to do this as I am running production. So what I want to do is pick up my edge in X and then add .002" to that value, is there a way to do that? My code for an edge find looks like this -

G65 P9023 A5. S54. (this picks up in the X plus direction)

I just recently found , through this forum I believe, that I can add a Q value to that where Q= the distance to travel looking for the edge. Is there another variable I can add to have it move the workshift after it picks up the edge? My machine is a Haas UMC-750, 2014 model. I know the above code calls up a 9000 series program and runs a macro in the background, I would prefer not to mess with any of that. Thanks for reading guys, looking forward to any help I can get.

You can just add to the variable # for that offset.

#5221 is the variable for G54 "X" (see the manual under system variables for a complete list)

so if you probe "X" and then want to move it +.010, just stick this in your program

#5221=#5221 + .010

Thanks for the response. I am not finding #5221, but I am not sure I am looking in the right place either (I looked inside program #9023). Let me clarify, I am not familiar with macros, I only know the probing routines from what is on the machine. I looked at the pdf for the inspection plus that came with the machine, but it seems outdated (not sure what version it is or what I have), or maybe the Haas is just different. The inspection plus shows examples of different probe routines like this -

G65 P9814 Dd (bore boss measurement)

G65 P9811 Xx or Yy or Zz (single surface measure)

But when I call these routines up on my machine they are in this format -

G65 P9023 A1. D1.5 S54. (picks up the center of bore and sets G54)
G65 P9023 A24. T25 H.01 (tool break check for tool 25 with a tolerance of .01")
G65 P9023 A5. S54. (sets G54 in the X plus direction)

So as I see this ^ the A determines the probe cycle, but I don't see any of that listed in the inspection plus pdf..? Is this something specific to the Haas machine? It seems all of my probe cycles use the same program (9023), and when I look at this program in the machine it does indeed seem to have headers like this ---> (x surface) (bore boss) (x web) etc. It seems all the routines are under this one program, does that sound right? Sorry if I confused the matter, just trying to wrap my head around some of this probing stuff.

Mike,

I'm relatively new to macros too. I'll try to explain it as best I can. The probing macros use what they call variables to store and adjust data. There are a couple of different types of variables...local and system being two types. When you run the probe routine to probe your G54 X-axis location, it stores that result in system variable number 5221. In a program you would use that variable with the pound sign #5221. What Larry said above is that if you put "#5221 = #5221 + .010" into your program the next line after your probe function, you will automatically move your G54 X axis offset .010" in the positive direction after your probe does its thing.

I'm not at my machine right now, but I believe you can see the different variables by paging through the Current Commands screen. See if #5221 is the same as the G54 X offset on your offsets page. That would be a good place to start.

Hopefully I didn't make this any more confusing,
Eric U

Are you probing every cycle? If not, #5221 = #5221 + .010 will move your X .010" every cycle no matter what. If you are probing every cycle, then this will work fine.

Seems like you may want to read up on G52 as well, depending on your circumstances.

At least on my '07 machine, readable variables only go to #999, so you're not going to see #5221. If you need to make sure it's working correctly beyond reading the code, you need to execute the code and watch your G54 location change in the offsets page.

Thanks for the help guys!

@Matt, Yes I am probing every cycle and I did see that I can only see the vars up to 999. I did indeed go with a G52 after reading that the Fanuc style parameter on the Haas for the G52 resets it to zero at M30. This solves my problem as I was always leary of using the G52 and then forgetting (or just not paying attention) it was there and screwing up the next time I picked up an offset. FWIW the Haas has 3 different methods of how it uses the G52.... Anyways, I did indeed find online a pdf tutorial of using the probe inside the Haas IPS and was clearly visible that there is (was?) a way to shift X and/or Y after probing a bore or whatever so I am not crazy.

edit: The xy shift was right inside the probe routine as shown, not a var you had to change elsewhere. I'm sure it did what you guys described and added whatever value you input, just was visible on the probing routine and not at another menu or screen.

May want to put G103 P1 prior to the probe, and G103 P0 after. G103 P1 sets the program look-ahead to one block. G103 P0 is the default, which is however many blocks the control is capable of looking ahead. Why do this? Well, I've had cases where I was doing math on variables and the control looked ahead and did the math before I was ready for it to. Caused the result to be incorrect. May not need it here, but after my experience, I've gotten in the habit of doing this anytime I'm probing and then doing math on the work offset variables.

Do you have the like 224 page inspection manual from renishaw? If not PM me your email and I'll send you a copy. I believe everything you want is in there, unless they changed something a bunch from the 2005 or so manual I have.

Its not that hard to write out all the macros, its just that you have to do one to spin probe on, one for protected moves then your measure macro, another protected move and then a spin off macro.

Just wanted to update my post. I found a newer version of the Renishaw manual (curious why I did not get the latest as my machine is a 2014 model?). To modify the X value (and I assume would work in Y the same way) you simply type it in at the end of the line. Super obvious, but I never even thought to try it, oh well, sample below for my Haas machine.

G65 P9023 A5. S54. X-.002 (picks up the G54 offset in the X plus direction, then offset it by -.002")

Note, the Renishaw manual says for the bore cycle it is I and J.

G65 P9023 A1. D1.5 S54. I1. J1. (picks up center of a bore, then sets G54 at X1. Y1. relative to where the bore was picked up)

hi guys, where can i find good manual for using macro programming on haas vf2 with renishaw probe?
I would like to be able to automatically do some things on each part in series, for example:

probe takes Y axis offset on the part on multiple points along the axis and then program calculates Y axis misalignment in degrees, then it automatically rotates B axis (we've got 5 axis tr160) to align Y axis correctly.

same thing for the Z axis, only moves A axis this time.

probe goes inside a hole and measures its diameter, if it's too small, the program repeats the tool which mills that hole but with smaller diameter, according to the error in diameter size.

Or, I'd like to check for tool breakage, for example after a mill finishes its cycle, it goes to measure it's length and diameter and if the value is smaller than defined from the last time it got measured, it automatically choses another mill from tool pocket and starts using that one instead of the first one, repeats the cycle and finishes the program with message that tool # needs to be replaced.

That would have to be a custom macro written by you. There is a tool breakage cycle but the machine will just alarm out. You'd have to write a custom macro for what you want there also.

yes but i need a manual or tutorial

I am new to the forum, but can anyone help with writing a program to check true position?
I run a Haas VF4 with the renishaw probe

eww an old thread.

MARK 1980 said:

I am new to the forum, but can anyone help with writing a program to check true position?
I run a Haas VF4 with the renishaw probe

Click to expand...

Take a read through here: https://diy.haascnc.com/sites/defau...ishaw_Programming_Manual_H_2000_6222_0A_B.PDF