Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

renishaw probe question


Recommended Posts

I have a renishaw OMP-60 probe and a Blum Z-nano ( Non Laser type )  tool setter. I have them calibrated and all of my tools always need to have a positive .0015 added to the respective tool length offsets page to have them blended properly. Is there a parameter on the machine control or something in the renishaw macros that I can add or subtract this .0015 difference so that when I touch my tools off they are one to one with my part pick up probe or at least a couple tenths at most. Just trying to dial them in closer than .0015 and not sure how to do it. The control is an Fanuc 18i-MB. Thanks for any helpful info anyone can provide.

Link to comment
Share on other sites

Got the fanuc books that tell you the macro info on where the memory positions are?

When you have that in hand then you can look at  the macro for calibrating the probe and see where its putting the information.

Of course if the macro is broken down into al kinds of sub calls it will be a lot harder to find it.

 

The other thing to do is very carefully go thru the calibration routine again but make sure everything is indicated in to .0002"

 

Machineguy

Link to comment
Share on other sites

When using the Renishaw tool setting macros, there is generally a #500 series variable that records the distance (in millimeters I believe) from the machine home position to the skip point on the tool probe, adjusting this number allows you to adjust the length that the touch off routine computes, sounds like its off by about .0015

 

Since the macro's are made to be able to use different variable numbers on different machines with different options it impossible to say with certainty what the exact number is.. but it's usually macro variable #520

 

If you think that's what it is and you are going to change it.. do yourself a favor .. make a small change and write your original number down before you change it!

 

 

Doh.. I am just editing this because I realized you said your using Blum laser so this wont apply..

 

Editing again to say I agree with the poster that said to lie about your tool offset length on your probe.. if you adjust your probe length it will change your results in Z when you touch off in Z

Link to comment
Share on other sites

Easy to solve, you just need to decide if you want to make the change in the tool setter, or the spindle probe. I don't have any Blum anything, so I don't know how you'd do it on that end.  But if you just want the spindle probe to match:  face off a part with a tool you just set on the tool setter, then run the 9801 calibration macro for the spindle probe, measuring on that surface.

 

Or skip all that, and just add/subtract .0015 to the tool length of the probe in your tool offset register and call it a day. 

Link to comment
Share on other sites

I have values for the probe from variable 500 thru 517 on the renishaw side. The blum tool setter is not a laser it's just a face that the tool comes down on kind of works like a TS27R but not as nice beings it's not renishaw. I have tried messing with the length offsets page on the register for the probe but I can set it to 1 inch off or .0015 and no change so it's not grabbing its number from the length offsets. Thanks everyone for the help.

Link to comment
Share on other sites

When using the Renishaw tool setting macros, there is generally a #500 series variable that records the distance (in millimeters I believe) from the machine home position to the skip point on the tool probe, adjusting this number allows you to adjust the length that the touch off routine computes, sounds like its off by about .0015

 

Since the macro's are made to be able to use different variable numbers on different machines with different options it impossible to say with certainty what the exact number is.. but it's usually macro variable #520

 

If you think that's what it is and you are going to change it.. do yourself a favor .. make a small change and write your original number down before you change it!

 

 

Doh.. I am just editing this because I realized you said your using Blum laser so this wont apply..

 

Editing again to say I agree with the poster that said to lie about your tool offset length on your probe.. if you adjust your probe length it will change your results in Z when you touch off in Z

 

 

 

I have the low tech Blum touch off that's just a round part on the probe each tool is touched off on. I can touch my part off then touch all my tools off but they are always .0015 above the area I touched off with my probe. that being said I have a work around, I just touch my part off then touch off all tools. then before running them I add the .0015 to my Z wcs on the control under my G54 etc. then when checking my tool blends they are all within a .0002. Im trying to take the extra work out so that the night shift operator with only 6 months experience can just touch his tools off and go and not have to mdi his tools to z- zero and blend them off accordingly. Also my variables are stored in the 500's in my control I just don't have a 520 value.  thanks for the info.

Link to comment
Share on other sites

On my Siemens controlled machines what I did was create a process in my post that applies a tool length offset shift based on a variable for every time a length offset is called.

 

So R100 = shift all tool lengths the same amount. Now that I think about it I never applied any error checking incase someone fat fingered a number. I should prob do that now.

Link to comment
Share on other sites

All the Fanucs with Renishaws (ts27r), I have setup have the "z adjustment number" in two variable places. Easiest way to find out what variables are relevant is to record macro variables, run calibration and see what changed. Its around 520 like previous poster said. Also, on your blum are you just plunging on the c/l of the disk? 

Link to comment
Share on other sites

All the Fanucs with Renishaws (ts27r), I have setup have the "z adjustment number" in two variable places. Easiest way to find out what variables are relevant is to record macro variables, run calibration and see what changed. Its around 520 like previous poster said. Also, on your blum are you just plunging on the c/l of the disk? 

 

Correct the with the Blum tools are just plunged to the center for tool touch off. I would rather have a TS27R but the Blum is what was installed in it. But I at least have a Renishaw OMP-40 part probe.

Link to comment
Share on other sites

Plunging with larger diameter endmills than the probe causes error due to the endmills center clearance. Does Blum have a manual setting macro to handwheel off center to pick up a single flute? We plunge on center with all of our probes. The higher powers didn't like the idea of the tools spinning on a carbide probe surface. Anyway, a 1/2 inch endmill on a 1/2 inch chamfered probe usually picks up a .001 error. I have seen 3/4's on the same 1/2 probe be off .003. I either just account for the distance or set it manually by hand wheeling off center line. If all the tools were being set accurately but just off the same amount, it would we a work coordinate issue. Blend issues are caused from errors in picking up large and smaller tools while plunging. And if the probe face is not indicated in. 

Link to comment
Share on other sites

Plunging with larger diameter endmills than the probe causes error due to the endmills center clearance. Does Blum have a manual setting macro to handwheel off center to pick up a single flute? We plunge on center with all of our probes. The higher powers didn't like the idea of the tools spinning on a carbide probe surface. Anyway, a 1/2 inch endmill on a 1/2 inch chamfered probe usually picks up a .001 error. I have seen 3/4's on the same 1/2 probe be off .003. I either just account for the distance or set it manually by hand wheeling off center line. If all the tools were being set accurately but just off the same amount, it would we a work coordinate issue. Blend issues are caused from errors in picking up large and smaller tools while plunging. And if the probe face is not indicated in. 

 

The macro I use has an option to offset the X or Y half the diameter of the tool in order to address the error for tools larger than the touch off pad. When touching off tools that large I always bring them down to a known surface in Z and adjust them as needed for the error if any in measurement. The tools I finish with are always less than the diameter of the touch off face which is 25mm I do believe. I also checked for flatness of the tool setter pad with indicator and its dead on.

Link to comment
Share on other sites

Our Hermle C40u's have the probe and setter as you and they are running within a tenth.  

 

How are you setting the standard and probe length? Off line or on the machine? The most accurate is to use a gage block and bring the spindle nose down to a slip/no shake, set zero and then probe the top of the block.  This compensates for the probe deflection. 

 

Make sure you use the radial offsets for the blume. the laser is at a slight angle and your error will increase as diameter increases if not. HTH's

Link to comment
Share on other sites

The manner in which I calibrate my probe depends on the machine it's on.

 

On a 5-Axis, I'll load the probe in the spindle, turn it on. Manually jog probe down to the table until it triggers. I know where that table is in machine coordinates, I'll subtract the machine position from the known position and that's my gage length. That gets me within .0003". Then I'll probe the position add the error to the probe's offset and call it good.

Link to comment
Share on other sites

Our Hermle C40u's have the probe and setter as you and they are running within a tenth.  

 

How are you setting the standard and probe length? Off line or on the machine? The most accurate is to use a gage block and bring the spindle nose down to a slip/no shake, set zero and then probe the top of the block.  This compensates for the probe deflection. 

 

Make sure you use the radial offsets for the blume. the laser is at a slight angle and your error will increase as diameter increases if not. HTH's

My Blum is not a laser tool setter. Its just a round touch pad that the tools touch off on the face of. I calibrate my part probe using the renishaw macro that came with the probe to calibrate the length of it. as for the Blum tool setter ( non laser) it came with a precision made and ground standard with the length laser etched into the side of it. That Value is used when calibrating the tool setter using supplied macro to do so. All off this calibration is done in the machine. I would be interested more in hearing better ways of calibrating my machines probe and tool length setter other than the supplied macros so as to tighten up the tolerances between them and my tools. I would love to have a .0003 tolerance would make my life a lot easier when I kick off 20 some paths to run unattended. thanks for all info provided. 

Link to comment
Share on other sites

Sorry, I missed the non laser in your original post.  

 

What spindle do you have in the machine?

Its a Toyoda FV1050S with a 15000 RPM spindle and a Fanuc 18i-mb control. really good running machine would just like to tighten up my tolerances of my touch offs

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...