Haas Probing cycle

Who here is an expert on probing with a Haas or Surfcam that might could talk me through setting this up? See the attached picture.

What we have is a tube thats machined with holes already. Well they had us weld up a few of the holes and the heat resulted in "egging" the part up to .023" on the ones we checked. Now they want us to come back and put .007 deep scribed indicator lines like you see in the drawing at each hole location. I am thinking this would be a perfect application to use a probe and the 4th axis to set a "z" work offset at each line location so the engraver does not go too deep.

Any help would be appreciated.

This is a little different from what you asked for, but thought I would post it anyway since it includes what you are looking for.

Have your Renishaw manual handy so you can reference what the different G65 lines perform.

Note: G54 will need a rough position for x,y and z to begin with. The probe will set the actual value.


Let me know how you make out.

(See Below)

-------------------------------------------

This program will set G54 X & Y offsets, then it will probe 5 locations in Z to set G54 through G58.
At the end of the program the values for G54 X,Y will be copied to G55 through G58
Haas Machines
%
O10000 (PROBE MULTIPLE Z OFFSETS)
(SETS G54 X,Y AND COPIES)
(VALUES TO G55 - G58)
(SETS NEW Z OFFSET FOR EACH)
G90 G40 G49 G00
G53 G49 Z0
T25 M06
G00 G54 X0.3 Y-0.3
G43 H25 Z2.
(PROBE ON)
G65 P9832
(START PROTECTED POS MOVES - P9810)
G65 P9810 Z1. F100.
G65 P9810 Z0.25 F50.
(SET G54 X,Y, S1=G54)
G65 P9811 Y0 S1
G65 P9811 X0 S1
G65 P9810 Z1. F100.
(SET G54 Z)
G65 P9810 X-0.2 Y-1.25 F100.
G65 P9810 Z0.4 F50.
G65 P9811 Z0 S1
G65 P9810 Z1. F100.
(SET G55 Z, S2=G55)
G65 P9810 X1. Y-0.3
G65 P9810 Z0.3 F50.
G65 P9811 Z0 S2
G65 P9810 Z1. F100.
(SET G56)
G65 P9810 X1. Y-2.25
G65 P9810 Z0.3 F50.
G65 P9811 Z0 S3
G65 P9810 Z1. F100.
(SET G57)
G65 P9810 X3.1 Y-2.55
G65 P9810 Z0.3 F50.
G65 P9811 Z0 S4
G65 P9810 Z1. F100.
(SET G58)
G65 P9810 X3.1 Y0
G65 P9810 Z0.3 F50.
G65 P9811 Z0 S5
G65 P9810 Z3. F200.
(PROBE OFF)
M53

G53 G49 Z0
(SETS X, G55-G58 = TO G54)
#5241= #5221
#5261= #5221
#5281= #5221
#5301= #5221
(SETS Y, G55-G58 = TO G54)
#5242= #5222
#5262= #5222
#5282= #5222
#5302= #5222
M30
%

You could also write a sub program that includes the probe cycle first then the engraving cycle. Then all you do is move, run the sub program, move, run the sub program. Should save you programming time. And your only working in G54. Should look like this:

o1

X0. M98 P2

X1. M98 P2

X2. M98 P2

M30



o2

G65 P9023 A9. S54.

(HERE IS WHERE YOU WOULD INSERT THE ENGRAVING)

m99

I omitted all the g90's and g43's and tool changes of course, and I used "X0., X1., and X2." as an example. You would insert your own X and Y coordinates for were you want it to probe and engrave. I actually do stuff like this all the time with my probe. You wouldn't believe all the cool stuff it can do. Setting offsets is just the tip of the iceberg.

The above recommendations are excellent and both will work with some specific editing on your part. Double a-ron is correct....this is very much just the tip of the iceberg. All Haas machines that are purchased with WIPS (probe and tool setter) have Renishaw Inspection Plus software running in the background supporting the VQC interface. This gives them a load of capability, but most Haas users do not know this functionality is present. You can also trade out the OMP40 probe for an OMP400 pretty inexpensively and then get full 3xis (and multi axis) probing capability. The WIPS package is 100% the best deal you can ever get on a probe and tool setter! As a Surfcam user, you might also like to know that there is a product available as an Add-In that will allow you to create you're probing programs from the Surfcam model. For your Haas, there is a product that enhances the Haas VQC interface and allows you to use much of the Renishaw Inspection Plus functionality that what VQC default allows. And still another product that allows inexpensive, complete SQL supported data collection and analysis from your probe...not Datamyte, Minitab or any of the other SPC programs. I'm already treading on the edge of advertising here, so I'd be happy to point you in the right direction, but it should be in a private message or over the phone to avoid breaking the rules of the forum.

So we just now got the machine set-up to try these suggestions.

So for my particular case in the above print where I want to hold the part in the 4th axis and I know where x-y zero will be for all offsets already and only need to probe the engraving locations should the program read something like this:

%
O10000 (PROBE MULTIPLE Z OFFSETS)
(VALUES TO G55 - G58)
(SETS NEW Z OFFSET FOR EACH)
G90 G40 G49 G00
G53 G49 Z0
T25 M06
G00 G54 X-3. Y0 A0
G43 H25 Z2.
(PROBE ON)
G65 P9832
(START PROTECTED POS MOVES - P9810)
G65 P9810 Z1. F100.
G65 P9810 Z0.25 F50.
(SET G54 Z)
G65 P9810 A10. F100.
G65 P9810 Z0.4 F50.
G65 P9811 Z0 S1
G65 P9810 Z1. F100.
(SET G55 Z, S2=G55)
G65 P9810 A20.
G65 P9810 Z0.3 F50.
G65 P9811 Z0 S2
G65 P9810 Z1. F100.

AND SO ON

Yes, overall you are correct with your program. I am assuming that your Z0 is not the center of the part, rather the actual surface you are engraving on. If that is correct, then your program is correct except for one item.

You will probably not be able to move your A axis with a 9810. In mulit axis applications, we normally need to "enable" skip on A, B and C axis with a special macro. So you will probably need to use a G1 or G0 to command the A positioning. Just double check your program to make sure your Z is clear. :)

Since you engraving its worth noting that your probe Length Offset is calibrated, but its also floating in releation to your other tools. For example, if you calibrated the probe a month ago and it was 68 degrees in your shop, your tool lenght might be 5.1234. But today, at 60 dgrees, it might be 5.1224 or some small variation. If your engraving tool was set today, then it would have the same relitive deviation. You might want to set the tools together...including the probe.... so they are relitive to each other, since you are using the probe length to set the WCS Z. Its usually easiest to run the 9832 and just touch the probe until it beeps or the light turns red on top of your tool setting standard. Of course, if your using a laser tool setter, this won't work.

Hope that helps.

Well I will probably just set it off centerline of the part and let it adjust from there. So I can use the G0 inside the probe cycle for the "A" command?

Working for center...fine. Your 9811's would then be Z1.395. Yes, you can use G0 or G1 whenever you like because your not actally burried in a macro cycle. Your program might look like this:

(START PROTECTED POS MOVES - P9810)
G65 P9810 Z1. F100.
G65 P9810 Z0.25 F50.
(SET G54 Z)
G1 A10. F100.
G65 P9810 Z0.4 F50.
G65 P9811 Z0 S1
G65 P9810 Z1. F100.
(SET G55 Z, S2=G55)
G1 A20. F100.
G65 P9810 Z0.3 F50.
G65 P9811 Z0 S2
G65 P9810 Z1. F100.

Something else I thought I should mention...when your using an S word in a probing cycle, you have switched the intention of the software from asking it "what a feature dimension is", to telling it "this IS what it is". So if you tell the software the Z size is 1.395 and its really 1.400, your WCS will still be set .005 off. Not an issue for what your doing, but important to know.

Are you referring to a line such as:

G65 P9811 Z0 S1

The 'S' is defining the work offset which is being set, is it not?

Where and when did Z1.395 come in to play for the topic? Did I miss something?

Quote:

---

Originally Posted by haastec

Are you referring to a line such as:

G65 P9811 Z0 S1

The 'S' is defining the work offset which is being set, is it not?

Where and when did Z1.395 come in to play for the topic? Did I miss something?

---

It came from using the centerline of the part up to the od. Is that not correct?

Yes...correct....S1=G54, S2=G55, S3=G56. S101 starts the extenced work offsets. Z1.395 is the radius of the cylinder he's working on. 2.790 is the diameter. If his work offset Z was set to zero as the center of the cylinder, then his probing Z would be G65P9811 Z1.395 S1. If the work offset Z zero is set to the engraving surface itself, then the probing would be G65 P9811 Z0. S1. as in his original example. It will work either way, just got to keep it all relative. :)

Thanks for the clarification Traceman and Probe Guy.:cheers:

I glazed over the print thumbnail when looking back and my train of thought was always with Z0 at the work surface since he was looking to hold a specific depth at each location.

Haastec- yop, you are 100% correct! I just felt it was also important to clarify and to point out that with Renishaw I+ (operating in the background on Haas), you don't necessarly have to be able to probe and X, Y or Z zero to be able to set the work offset. Great points....thanks for the input!

Traceman- hope the engraving works well for you.

Well I just got done with it and it worked great. Don't know why my guys never use it. It sure makes setting up a lot easier.

Thanks for all the help guys!!

LOL...yep, therein lies the great mystery that cause this company to be created....why do shops spend thousands on these devices and not use them? We are finally starting to change that. If you need any more help or want to see what else you can do with that probe, just drop a line. Glad it worked for you!

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.

I have a 6 station fixture in a UMC-1000. the stock for this fixture is 6" OD 4" ID by 5 inches long aluminum tube but came in all over the place size wise. i would ideally like to set the machine up to probe each bore at the beginning of the program but i dont have alot of hand programming experience. would you point me in the right direction for how to do that.

Not sure if you still need help with that 6 part problem on your UMC but lmk if you need help figuring it out.