Renishaw laser

[Bill]

We just got our new Hurco (don't laugh) and they went with the Renishaw laser to help eliminate operator error (don't laugh).

 

The tech guy they sent out didn't know how to answer my question.

 

Here is what I asked...

 

My boss wants or intended on us using the laser to verify tools before and after cuts before a tool change is made to see if cutter held up. How or where do I begin to get that into my programs?

 

The tech didn't know if it was a gcode command or not and he didn't know where I would put it in.

 

Do any of you use this? If you do, could you please give me some guidance?

 

Help is much appreciated.

 

Thanks

 

Bill...new to this laser stuff.

[crazy^millman]

Is if a laser for probing? If so then you would be putting in the probe during a toolchange and it only work when changing tools to that probe so you could never measue a tool before or after since you need it to do so. Now if it is a auto detech laser then you should have a Code be it G or M though I would think it would be an Mcode that you would use before the toolchange like a ref point or point in Mastercam ot go to then use the Mcode the check the tool for Breakage. Now if it is for toolbrakge it is not going to tell you wear. But if you got a touchsetter type toolprobe then you need the machine to have tool libary and tool life managemtn capabilites which is a horse of a different color. You need the abaility to montior offsets such as length, wear or diameter. Then you need the system to have acceptable tolerances in which is uses to gauge what is a good critea for that tool. I would think that you could do a time study type of checking where you know so many hours and this tool is toast or you could go wit ha horsepower change to get the tools life or a diameter change, I perfer the Horsepower change on roughing tools verses time, I like time or actually tool or part measurement verses horsepower on finishing becuase almost never use any horsepower to finish. So not only are you in need of a awya to measure the tool but you are in need of more if you want to be effictive at doing it IMHO. The concept tis a sound concept but does the machine have all of that I would not know and if your TECH help is limited to a Code then answering the rest of that is going to be a old good luck.

[Bill]

Thanks Ron,

 

Yes we were basically looking for a way to see if the tool is broken before sending in smaller cutters. Instead of coming in in the morning to find the 1/4 ball broke first then the 1/8 etc.. etc..

 

I would suspect tech is limited. At least as far as the guy they sent out to "train".

[iowajim62]

billh,

quote:

---

Cost effective, fast and reliable, the single-sided device can detect tools as small as Ø0.5 mm, with the tool typically spending about 1 second in the laser beam. The TRS1 uses Renishaw software, specifically written for, and supplied with this new product.

---

from Renishaw web site. Looks like you need software installed if this is what you have.

Their Probes use 1 line G-codes, maybe the lasers do too.

 

http://www.renishaw.com/client/category/UK.../CAT-1079.shtml

 

Good luck and I wasn't laughin at ya

I was laughin with ya

[[email protected]]

Bill,

We also have a Hurco with the laser option, and Hurco told us that until there next update (which is also a hardware update) it will only do tool management in conversational programs. I bet that wasn't in your sales brochure.

[Bill]

Uhh No it wasn't.

 

I have been reading on Renishaw's site. Will see if the macro program they have for tool breakage is available for Hurco which I think may be the same as Yasnak.

 

Thanks guys.

[medaq]

I know this is of a different topic, But atm we are having our laser ripped out of the machine to place in a new touch style sensor. We have found way to many problems with the laser systems.

 

One is coolant drops through the laser can screw up the reading especialy if 2 drops break the beam during measurement.

 

Atm we have been tracking .005 variance with our laser. I set a little macro program to pull in a gage pin to measure after every pallet change. And the numbers are all over the place for us.

 

Personaly I was very optimistic for the laser tool probe but after 6 months of agony I am not. Just for tool breakage it could be pretty nice. But still alot of problems will arise out of it imho..

 

 

Jim

[Guest CNC Apps Guy 1]

What I do is check the tool AFTER an operation. This is sufficient because if you ALWAYS check after and it checks good, then unless somebody took a hammer to the tool while it was in the carousel (Don't laugh, I've actually heard of this happening) it will be good.

 

Then if it checks bad you stop the program.

 

This is easy to setup in the Post (at least for me as I've done it for a dozen or so different posts).

 

Jim, is this on a Horizontal by any chance? If so, before you rip it out, let's talk. I've seen some issues in horizontals resolved before.

 

I've been able to repeat ±.001 or better depending on the tool on the one I am setting up at the moment. If your checking macro does not do thermal comp, you'll have issues.

 

JM2C

[Chris Flint Two Ft Pty Ltd]

I like James's idea, could you not just use a tool setting probe mounted somewhere on the table and when a machine path is finished, (write a small program to make the machine go to the tool probe and) check the reading if no reading stop machine cycle

[Bill]

James, that is what I am looking for. Renishaw uses macros written into your controller.

 

example they show is...

 

Format G65 P9863 [Hh Mm Ss Yy Zz]

where [ ] denotes optional inputs

Example G65P9863 H5. M1. S2800 Y3. Z6.

 

BUT I still can not verify if this macro will work with this Hurco.

 

They have something in the appendix that states...

 

Appendix B Yasnac controller settings

The Yasnac range of controllers – MX3, J50, I80 and J300 – use a

different configuration of tool offset options to those used by Fanuc.

There are no separate wear and geometry registers.

 

Not sure if this means it won't work.

 

I do have another question that arose at the end of the day yesterday about the post. I am going to start a new topic for it though. Kind of a funny story to go with it...I'll put that in O/T.

[medaq]

quote:

---

Jim, is this on a Horizontal by any chance? If so, before you rip it out, let's talk. I've seen some issues in horizontals resolved before.

 

I've been able to repeat ±.001 or better depending on the tool on the one I am setting up at the moment. If your checking macro does not do thermal comp, you'll have issues.

 

JM2C

---

James, Yes it is on a hplus 300 horizontal. I wish I could see .001 at this time. We have been fighting this new machine for 6 months now. We have the nc1 laser probe on it currently. I love the idea of the system but after pulling our hair out for the last 6 months I am becoming sour to it. As for the thermal comp in the macro I need to look into that portion. The guy who installs the renishaw does not want to do any more tests to it. As for him he says it works as intended. Of course I say a .005 varying offset is working as intended?

 

But the problem is he has been paid and does not want to put fourth any more effort to our problem. Atm the machine tool builder is paying for a coolant chiller and is being shipped out to see if this helps with out accuracy issues. We did find one thing, their thermal comp was not compensating the machine correctly. And has been tuned in but I am worried that since they tuned it in with no coolant. That when running coolant it will have a big change.

 

Anyhow if you have any ideas on the probe, please by all means I will try anything. Seems like all the guys I get have very limited knowledge on how tomake it work correctly.

 

Jim

[medaq]

quote:

---

BUT I still can not verify if this macro will work with this Hurco.

---

Hey bill,

 

Are the macros installed in the machine? Or are you having to do install them your self? If you are installing everything dont forget to align the laser through macros. I think you need to run 9860 for beam alignment and 9861 for the calibration. I am pretty sure the renishaw macros are pretty universal. But might want to varify that.

 

I wish I had a better answer for you, But unfortunately never had my hands on a hurco.

 

I can comment on some of my solutions to implementing a tool check. Can do it one of 2 ways pretty easy enough. One I hand type a manual entry into mastercam, so mastercam will spit out the code to check the tool. Now my machine has macro #517 which is basicaly the head tool number so it allows me to have one standard macro line check the tools.

 

G65P9862B1.0H.025T#517 to set

G65P9863B1.0H.025T#517 to check.

 

If you do not have a #517 like me, just replace that with the tool number.

 

You mentioned checking the tools before and after. So if you are going to always check the tools, You could also embed it into your tool change macro.

 

Just one thing to note if you want to set the tool, It is better to use the y shift for the tool. Since this will break the beam in a smaller spot so when checking from tool to tool you break the beam in a more constant spot.

[Bill]

Thanks medaq,

 

the macros should be installed already if the hurco controller is capable.

 

I will find out Monday.

 

Outta here for today.

 

thanks again everybody.