Bore ID measurement with Renishaw Probe
Is it possible to make a program to have a renishaw probe measure a bore diameter? I have a renishaw probe that came with a Hass VF mill, it has the macros for finding work offsets, I wasn't sure how difficult it would be to make a program to find a bore diameter. My tolerances are not tight, I'm looking for +_.001.
Anyone know of a 3 point bore gauge that is reasonable? This is for a 3.54' ID
You need the software to do it. yes it can be done. I have the Renishaw probe as well on my Mazak VTC. I cannot use it as a measuring device cause I don't have the software but you can buy the add on and it definitely can be done.
Yes, there is a macro for measure its very easy to write you need the book it shows you how.
Not true for Haas machines that came equipped with a probe.
Originally Posted by Hertz
Tyson, send me a PM with your email address and I'll send you both OMP-40 and TS27R manuals. Measuring a bore is dead simple.
Ok. With my machine, the software is an option. I guess with Hass, you get it included. My Mazak was purchased with the probe as well but THAT part was not included. I can certainly probe a hole, it just doesn't measure it for me.
I'd rate this task as not hard at all if you know how to write macros.
That said, I have a big problem using the machine that made a hole to inspect it.
Controlling size, comping for tool wear fine. An actual part measurement, no way I'm going to try this.
You need an outside gauge to verify the machine's zero numbers.
Cutting machines are not measuring tools and the two are designed differently.
Think about something simple like a bad screw bearing on one axis.
If the machine has a problem and is making the wrong size it is going to make the same mistakes when measuring.
I've had a $650,000 grinder happily gauge, comp, and make scrap parts all day long.
There is no way in hell I would trust any machine to final inspect it's own parts.
(Post warning, I build process gauges so my opinion may be a bit skewed.)
+/- 0.001 can be measured with a Mitutoyo dial bore gage with a tenths indicator. You'll need a 3-4" micrometer as well and preferably also a gage block close to 3.54".
Originally Posted by twitte
If you have a Haas with the Renishaw probe factory installed then you can easily measure a bore. It will measure to whatever the capabilities of the machine are. You also have the ability to do a 3 point bore measure where you define what 3 points to measure, though if you are using the Haas VQC to calibrate the probe you will need to make one edit to the macro and recalibrate the probe before using the 3 point bore measure. If you contact Renishaw they can email you a copy of the manual for the probe programs.
Haas machining center equipped with Renishaw software can be used as measuring device. After each cycle the results are stored in macro variables. The size of the feature is always stored in variable #188 (in Haas).
3 point measurment is a bit tricky, as you have to calibrate the probe using different routine. But if your tolerances are as mentioned - just disregard that. The result will be good enough with standard calibration too.
In order to execute it position the probe close to the center of the bore and run the following command:
while A, B and C are the angles at which you want the probe to touch the circle (0 degrees at 9 o'clock, CCW).
At the end of the cycle you will find the actual diameter in #188, and X and Y center coordinates (in current coordinates system) in #185 and #186 respectively.
The closer your initial position is to the real center of the circle, the more accurate ar the results. When looking for high accuracy, I suggest to make several attempts, each time updating the start point according to results in #185 and #186.
I gave this a whirl and got a Probe open alarm...
Originally Posted by PROBE
Any insight into what I did wrong..
This is the test program I wrote to measure the true location of a hole that is 4 inches away.
It would seem safer to feed that probe down into the work with it armed too... Should I add a line to arm it? If it is armed will it stop any time it makes contact?
Arming is M59P1134 correct?
I would love to learn how to use this new machine and probe to pick up hole locations in die plates and such when the time comes for rebuilding smashed stamping dies...
You forgot to switch the probe on. Change your program as follows:
Originally Posted by ARB
G65P9832 (PROBE ON)
G65P9833 (PROBE OFF)
As to your new task, do you want to set individual WCS for each of the holes in your plates ? If yes - what WCS numbers ?
On my first go round I used the Haas IPS to set a WCS for each hole then did the math.
I was just trying to learn how I might use it to output hole locations or true center distances. Poor mans CMM for reverse engineering old stamping dies built without a DRO on manual mills.
Turning the probe on is a good plan.. Thanks
I take it that if I want to inspect several holes I can just copy the #185 and #186 to one of the #500 variables to store it until I am done.
Originally Posted by ARB
What will you do with the results once stored in => #500 Variables? Alternatively, you could output the results, as and when obtained, to a PC File using DPRNT.
Depending on how new your Haas is, you can have it output the diameter measured in the probe bore cycle right on the screen. If you have the control that has multiple "menus" displayed on the screen i.e. positions, program, spindle speed, etc. Probably 2011-2012 or newer I would guess. Anyways, in the current commands you can assign macro label #1 as variable #188 and it will output the value of #188 in the lower right corner of screen. There is a small box that has "Label 1" and "Label 2". FWIW #188 (on my particular machine, umc-750) apparently measures "y" as you will get a measurement in label 1 for probe bore, probe rectangle (y width) and I think pocket "y".
Does anyone know what value outputs the "x" in this scenario? I checked my inspection plus book but apparently it is out of date as it has the bore measurement as #136 or something, not #188, which is working on my machine....
I have a 2013 haas vf4-ss with the probe. Go into your probing (where you use the probe to set work offsets) go to probe bore. Put the probe close to the center of the bore. Tell it the diameter and it will probe it in 4 places. After it probes it, it automatically centers the probe to the center of the bore. So I run it again now that it will be more accurate. Then go to you macros and like other people said, #188 is the diameter. I have found mine to be within a couple tenths.
I thought I read somewhere this is a new Haas for you? You really shouldn't have to write anything (other than what you want for custom cycles). You should have quite a few probe routines stored in the machine, you just enter variables such as approximate bore size, x&y widths, z moves, etc.
Originally Posted by ARB
Thanks guys. The machine is brand spanking new. Up until now I have only used the probing to set offsets.
There could be more documentation for the probing.
PM me your email address, I have the renishaw manual on pdf