Calibrate Renishaw probe length on Brother

[Peroni]

I am totally lost on how to calibrate the stylus length on our Brother M300X3. We just had a Blum tool setting installed yesterday and that is working but when I try to use the Renishaw to probe the part I get a message saying to calibrate probe. Have a calibration ring to do XY but I have never done Z nor seen it done. The Renishaw manual for Brother is less than helpful. I also cannot make sense of the procedure in the Go Probe app. Probe in the machine is in pot 22 but is labeled as tool 99. Help?

 

[BROTHERFRANK]

Did you purchase the machine through Yamazen Knoxville? Did you purchase the probe with it? If so, installing and calibrating is not your responsibility. It should be done by the installer/trainer and you should be trained how to use it. Have you contacted your local support and sales rep? Let me know if you need further assistance please.

 

[Peroni]

The machine was purchased thru the Knoxville branch and was ordered with the Renishaw spindle probe. That was over a year ago and the probe had been working fine. Yesterday we had a Blum tool setter installed and now that works but the machine is saying I have to now re-calibrate the Renishaw which I have no idea how to do. It's not straight forward like on our HAAS machines. I sent a message to the guy who installed the Blum yesterday as well as our local app guy but haven't heard back from either yet.

 

[BROTHERFRANK]

got it. I will check with your local team.

 

[Luke.kerbey]

I’ve always known a probe length to be a positive figure measured from the spindle reference to the top of the probe.

Can you view the probe in the tool library which shows its length?

If you can edit this number manually, you may be able to set the spindle reference on to a stack of slips or parallels by the following procedure.

First set the spindle reference on to a stack of slips then, zero off.

Then call the probe, activate it and manually bring it down on to the stack of slips and find the trigger point using micron increments.

Read the z number (maybe around 150mm) and input this in to the tool library for the probe.

Then to check the setting, probe any surface, like the back of the vice if it’s ground, and then bring up a tool with a known good length and position it 10mm above the back of the vice and see if the 10mm slip fits. Then make very minor adjustments if needed from there.


Your machine may not have a full procedure for this because what I’ve written above is just as easy to do and may have been the intended way.

 

[Peroni]

It's well and truly stuffed mate. Service tech will be out Monday. So frustrated with this machine. Love our Speedio to bits but have none for the M300 - yet....

 

[gkoenig]

Aside from the probe calibration bits - which is more a Renishaw thing than a Speedio thing, what else about the M300 has made you not love it?

 

[couch]

More than likely what happened is they installed the Blum toolsetter, with the Blum tool setter cycles and calibrated it’s location using macros #510-514. Problem with this is Renishaw uses #500-519 for the spindle probe. So tool setter calibration over wrote the spindle probe calibration.

Have them change the tool setter macros to anything else, then recalibrate the spindle probe XY in a ring gage. The program should already be in your machine. The Z is taken from the tool length offset for the probe, it’s not calibrated like XY is. Once the probe length is touched off, set a Z work offset on a gage block stack and adjust the tool length offset to compensate for any error you’re seeing in the Z offset result after probing.

More than likely your Z is fine already, it just needs the XY recalibrated.

Do you have program 8028 in your machine? If so check to see what macros it’s using. If it’s #510-514 they’ll need to be changed, and the macros within programs 8001 & 8002 will need to be changed to match. Edit those first, run 8028 to populate the macros, then run XY calibration for the spindle probe and you should be good to go.

 

[Peroni]

Aside from the probe calibration bits - which is more a Renishaw thing than a Speedio thing, what else about the M300 has made you not love it?

IDK our HAAS and Robodrill machines have much simpler calibration routines than this M300. Maybe it's a multiaxis thing?

Biggest gripe with the M300 is lack of Z where it's needed. Spindle will only go down to about level with the Y way covers. Tilt the platter 90° and you best be working on a part 6"+ or you will end up with gage lengths in excess of 8" to work on small stuff. How the hell am I supposed to do any milling at all like that? And while having the trunion's main range of tilt back toward the machine makes for a shorter footprint it totally hides the work so you're totally blind if something is fucking up. Tools are harder to load than the Speedio. Interior lighting is mediocre at best. Our machine has a belt conveyor and coolant constantly splashes out around the opening for it. I'm also finding support to be rather poor compared to the Speedio. We purchased the G54.2 option only to find no one at our branch knows how to use it. I've yet to be contacted by anyone from Yamazen who actually does know something about it. So we abandoned it for G68.2 but again haven't found any local support for it. Thermal comp sucks but it does on our Speedio too so I won't hold that against the machine but it's something to be aware of. I think for a specific part it may be a great machine but it sucks in a job shop environment. Let's just say I'm glad it wasn't my money spent on this thing. I've been trying hard to want to really like this machine but I've been hit with frustration at every turn, mostly with regards to work envelope. Having it down for a week just to install a tool setter and then not even being able to calibrate a dumb spindle probe is not helping.

More than likely what happened is they installed the Blum toolsetter, with the Blum tool setter cycles and calibrated it’s location using macros #510-514. Problem with this is Renishaw uses #500-519 for the spindle probe. So tool setter calibration over wrote the spindle probe calibration.

Have them change the tool setter macros to anything else, then recalibrate the spindle probe XY in a ring gage. The program should already be in your machine. The Z is taken from the tool length offset for the probe, it’s not calibrated like XY is. Once the probe length is touched off, set a Z work offset on a gage block stack and adjust the tool length offset to compensate for any error you’re seeing in the Z offset result after probing.

More than likely your Z is fine already, it just needs the XY recalibrated.

Do you have program 8028 in your machine? If so check to see what macros it’s using. If it’s #510-514 they’ll need to be changed, and the macros within programs 8001 & 8002 will need to be changed to match. Edit those first, run 8028 to populate the macros, then run XY calibration for the spindle probe and you should be good to go.

Yeah we got the probe data storage locations sorted out and the Blum recalibrated, no issues there. The Renishaw was/is all kinds of messed up. I was able to get XY calibrated properly but no luck with Z. It does not help that the process to do Z is rather convoluted and confusing. I was finally able to get Z calibrated but it's not right. If I try running the routine with what should be the proper numbers I get Z over travel alarm. We had issues with the probe not working at all right from day 1 so there may be a larger issue at play. I never really used it much as none of the included probing routines ever worked. Only the Go Probe routines worked and it was so clumsy to edit them all the time I just used the 3D Taster from our Speedio to set up. Service tech will be here Monday to hopefully sort things out.

 

[couch]

We purchased the G54.2 option only to find no one at our branch knows how to use it. I've yet to be contacted by anyone from Yamazen who actually does know something about it. So we abandoned it for G68.2 but again haven't found any local support for it.

I don’t work at Yamazen anymore but here are a couple threads where I’ve talked about G54.2, how it’s used and how to get it to work with probing. The parameters should already be setup in the M Series. Just adjust the axis compensation in the RFO tables to AC instead of just A.

Last page for the setup/format.

New Machine(s) Day! Brother S700X2 and Hardinge GT-27SP

Probing macros/routine to populate the Rotary Fixture Offset table.

Brother S1000 4th Setup

All the probing cycles I’ve mentioned are Blum, not Renishaw. IMO they’re way cleaner and easier to use so might be something to look into swapping to instead of Renishaw.

 

[gkoenig]

Yeah we got the probe data storage locations sorted out and the Blum recalibrated, no issues there. The Renishaw was/is all kinds of messed up. I was able to get XY calibrated properly but no luck with Z. It does not help that the process to do Z is rather convoluted and confusing. I was finally able to get Z calibrated but it's not right. If I try running the routine with what should be the proper numbers I get Z over travel alarm. We had issues with the probe not working at all right from day 1 so there may be a larger issue at play. I never really used it much as none of the included probing routines ever worked. Only the Go Probe routines worked and it was so clumsy to edit them all the time I just used the 3D Taster from our Speedio to set up. Service tech will be here Monday to hopefully sort things out.

Step 1 is ditch the stupid Renishaw macros. Rennishaw attempts to get macros to do literally everything, so they are far too complicated and convoluted. This is why they had to write an iPhone app to help people structure their macro calls. This complexity and the structure makes them a bit wonky sometimes.

Yamazen has their own macros, with a nice manual. They are extremely straightforward to use and I've never found a situation where they don't do everything I need them to.

On an M200/300, what surface is used as the reference for Z0? The top of the table at A0 B0?

 

[couch]

On an M200/300, what surface is used as the reference for Z0? The top of the table at A0 B0?

Table surface at A0 is Z0. This is 30mm below centerline of the A.

 

[Rick Finsta]

To calibrate Z you need a known length tool. I use the Maritool standards but you could also use a dowel in a holder if you have an offline tool setter?

Otherwise you can use a dual contact holder with the dowel method and the gauge line is a known distance from the flange. I can look up the number if you need - I have it somewhere around here.

 

[Luke.kerbey]

Rick, You don’t need an existing tool to work out the probe length. It’s a simple measurement from the spindle reference face to the probe tip that will equal the length.

 

[couch]

Known tool length is just for calibrating the tool setter. With the Renishaw macros you just need to touch off the tool on the tool setter and it’s done for Z calibration. The programs pull from the tool length offset. Any adjustment in Z work offsets (checked by touching off Z on a gage block) is adjusted in the tool length offset.

The Blum/Yamazen cycles have a calibration cycle for calibrating Z.

 

[Luke.kerbey]

Couch, that will only be as accurate as the tool setting calibration it self.

 

[PROBE]

Known tool length is just for calibrating the tool setter. With the Renishaw macros you just need to touch off the tool on the tool setter and it’s done for Z calibration. The programs pull from the tool length offset. Any adjustment in Z work offsets (checked by touching off Z on a gage block) is adjusted in the tool length offset.

The Blum/Yamazen cycles have a calibration cycle for calibrating Z.

Calibrating the spindle probe on tool setter probe is, per definition, inducing error, as 2 spring loaded devices are pushed one against the other. It is obvious that the trigger is generated while both springs are already squeezed, nobody knows how much.
The proper way is to calibrate on surface. This is what I recommend to my customers:
1. Place piece of material (aluminum) on the table or in vise.
2. Fetch just measured on tool setter end mill (0.5 inch or so)
3. Using the handle lower the spindle toward the material, start the spindle and take thin cut about 1 inch long in X or Y. DO NOT RAISE THE SPINDLE ! Set Z WCS in for example G54. The straight forward method is: Observe the Z machine coordinate (negative number, let’s say -10.250). Fetch the used tool length from tool offset register (let’s say 2.5). Calculate: -10.250-2.5=-12.750. Dial the -12.750 to Z register of G54.
4. Change tool to probe.
5. Using the handle place the probe tip some 0.25” above just machined surface.
6. Execute this small program:

%
G54
#100=** (PROBE TOOL NUMBER, EDIT ACCORDINGLY)
#101=#5023
M## (SWTCH THE PROBE ON, EDIT ACCORDINGLY)
#3004=2
G91
G31Z-1.F20
G0Z0.15
G31Z-.5F1
G4
#[10000+#100]=0
#[11000+#100]=#5063
G0Z[#101-#5023]
#3004=0
G90
M%% (SWITCH THE PROBE OFF, EDIT ACCORDINGLY)
M30
%

The probe length has been loaded to tool offset register.

Stefan
Cogito Ergo Sum

 

[Luke.kerbey]

I like the comment about two sprung loaded interferences, I hadn’t thought about that.

But what would you suggest if you don’t have a presetter? Or a existing tool with a known length?

 

[gkoenig]

I like the comment about two sprung loaded interferences, I hadn’t thought about that.

But what would you suggest if you don’t have a presetter? Or a existing tool with a known length?

Make a tool of known length...

1- Take the empty spindle and hand-wheel it down to the table.

2- Use a couple of 123 blocks and slip fit them under the spindle as if you were touching off a tool in the old-school methods.

3- Zero out your coordinates (operator coordinates, DRO, whatever they are called on your control).

4- Put a tool in the spindle, preferably a decent size end mill.

5- Slip fit the 123 blocks under that tool and read your DRO - you now have an accurate tool length.

The bougie thing to do is use an end mill holder with a gauge pin to make a permanent length standard to calibrate everything off of. One nice thing about this is you can drive this tool to sort of a "logical" value above the 123 block set (say 5", or 4.5" or whatever), and loosen the set screw to let the gauge pin extend to the top of the 123 block set. It is very nice to have a calibration tool with an easy to add/subtract value, and you should definitely have a permanent gauge.

 

[Luke.kerbey]

Make a tool of known length...

1- Take the empty spindle and hand-wheel it down to the table.

2- Use a couple of 123 blocks and slip fit them under the spindle as if you were touching off a tool in the old-school methods.

3- Zero out your coordinates (operator coordinates, DRO, whatever they are called on your control).

4- Put a tool in the spindle, preferably a decent size end mill.

5- Slip fit the 123 blocks under that tool and read your DRO - you now have an accurate tool length.

The bougie thing to do is use an end mill holder with a gauge pin to make a permanent length standard to calibrate everything off of. One nice thing about this is you can drive this tool to sort of a "logical" value above the 123 block set (say 5", or 4.5" or whatever), and loosen the set screw to let the gauge pin extend to the top of the 123 block set. It is very nice to have a calibration tool with an easy to add/subtract value, and you should definitely have a permanent gauge.

Why go through the process of making a known tool when you can just do the same thing with the probe? Or am I missing something?