What's new
What's new

Renishaw and the cutter diameter conundrum: the offsets holy war

A picture and a thousand words, etc. Can you tell I used to live and die by PowerPoint? :D

lets say i need to finish machine a .55" bore with .5" endmill (i know in practice this is a bad idea), theres basically no way to get cut comp to work here?
I gave this a lot of thought last night. I can't think of how to make this work using Diameter and not sure wear would work either. The problem is you need to arc into the desired ID circle because you're inside. You can't use a tangent line to merge onto the geometry.

With that said, Mastercam has an option in at least some of the cutter paths that allows you to establish cutter comp above the part. You could lead in on the cutter path for 6" if you wanted to, start a spiral, feed down into the bore and retract out before cancelling cutter comp. I've never tried it but, seen it.

And to add some confusion (or not): on the last slide, I exaggerated what the cutter start position would look like (being way off the line). If Mastercam knows you have a 1" diameter cutter, it starts the first position 0.5" away from the line. It would look the same as if you weren't using comp at all. It then does the compensation, on-ramp, merge thing. Except: I'm already merged. The 'calculated path' tapers but, the cutter looks like it follows the line straight in to being fully compensated. Again: this is why people argue back & forth because the CAM software makes both methods somewhat seamless.
 
I gotta give Donkey props, time is a our most valuable commodity.
He spent time, researched some stuff, and built some visual learning aides,
Donkey's observations is good. It's his conclusions that are suspect :D

Donkey Hotey said:
I can't think of how to make this work using Diameter and not sure wear would work either.
That's why you skip all this newfangled cutter comp crap and just run 'er through the interpreter again, get the cl you need :D
 
That's why you skip all this newfangled cutter comp crap and just run 'er through the interpreter again, get the cl you need :D
Truth is: most things I've ever made were crazy low quantities--usually 1-5 pieces. I do / did exactly what you're saying. I do use the measured cutter values that the Renishaw comes up with for actual cutter diameters in Mastercam.

I was working on someone else's dime and played with all these methods though, because my own interest was designing repeatable processes.

That included being able to have a low skill person change a cutter (or me change a cutter in a hurry) and get back to cutting parts on dimension quickly. That's why I wanted it to use the turn-key Renishaw presetting macros.

Similarly: a production process might include optional Block Delete lines for tuning wear offsets: in Block Delete mode, stop after a cut, probe the dimensions just cut, adjust the wear column for that cutter, then resume / finish cut that feature. This could be switched on by the operator to automatically do the tuning on this cycle and turned off when the process is giving good parts reliably.
 
my own interest was designing repeatable processes ... That included being able to have a low skill person change a cutter (or me change a cutter in a hurry) and get back to cutting parts on dimension quickly.
So here's a thought. These things even from haas are like eight grand. Yes it sounds like a lot when you can tie up your machine for hours a week touching off tools instead but ... this is semi-speculation but I'd be willing to risk a $50 bet that a tool presetter pays for itself pretty quick, even at the heart-attack (damn I'm cheap) prices.

IMG_5900.jpg

and ya know, haas, local "service and support" and all that stuff. They'd probably even put it on the time payment plan.

And if people insist on talking tenths, well, laser optics are fairly accurate. Angstroms or something, I dunno ...
 
So here's a thought. These things even from haas are like eight grand. Yes it sounds like a lot when you can tie up your machine for hours a week touching off tools instead but ... this is semi-speculation but I'd be willing to risk a $50 bet that a tool presetter pays for itself pretty quick, even at the heart-attack (damn I'm cheap) prices.
But again: I wanted a whole process to just work, right in the machine:
  • Take out this cutter
  • Get another from the bin
  • Install the cutter
  • Torque to 80 ft/lbs
  • Turn on Block Delete mode and press cycle start.
Machine verifies the tool length and diameter against the old one (or the program). Machine probes the part for interim final dimension. Machine changes wear offset. Machine cuts finish pass.

It could run like that all day (slowly re-tuning the wear offset) or turn off Block Delete and skip the probing until the next tool replacement.

Thinking way ahead: I wanted to write the custom wear-tuning macro to run like the other Renishaw macros. Pass the tool numbers, locations and dimensions to the macro in a single G65 line. That way it could be used in any program and would only need a single Block Delete to switch it on and off.

Probe X web, Y web, X pocket and Y pocket are the same macro. They decide what they're doing by which variables are passed to them in the G65 line.
 
I gave this a lot of thought last night. I can't think of how to make this work using Diameter and not sure wear would work either. The problem is you need to arc into the desired ID circle because you're inside. You can't use a tangent line to merge onto the geometry.

Come on Donkey!!!

G00 X0. Y0.
G01 Z-0.5 F50.
G01 G41 X0.02 Y-0.255 F10. <--- Ramp onto lead-in arc
G03 X0.275 Y0. I0. J0.255 <--- Lead-in arc of .255R
G03 X0.275 Y0. I-0.275 J0. <--- The .550 dia bore
G03 X0.02 Y0.255 I-0.255 J0. <--- Lead out arc of .255R
G01 G40 X0. Y0. Z1. F200. <--- Ramp off lead out arc.

To think about it in another way, the built-in G12/G13 command does that automatically!

Also, one of your slides is incorrect a bit.
The "minimum length line" slide is wrong
You're asking a 1" endmill to make a .35 step while on profile. That is an absolutely possible move, and no control will barf at it one single bit.
Just run this and find out for yourself:

(1" cutter, offset table is set to 1" dia )
G00 X-2. Y2.
G01 G41 X-2. Y.35
G01 X0 Y.35
G01 G01 X0 Y0
G01 X2. Y0
G01 G41 X2. Y2.
 
Come on Donkey!!!
I don't know. I'd have to draw this out. He said a 0.5" cutter in a 0.550 hole. Not a lot of room to back up and get a run at it (even with Wear). You're right, there are other ways to do it.
Also, one of your slides is incorrect a bit.
The "minimum length line" slide is wrong
You're asking a 1" endmill to make a .35 step while on profile. That is an absolutely possible move, and no control will barf at it one single bit.
Just run this and find out for yourself:
You might be correct on this. All six slides were off the top of my head. I think it may still choke because the cutter never touches the vertical line. CADAM used to gag on that. Dunno about the Haas and that's all I have access to. I'll trust that you've tried it and it worked.

I can think of other examples that would fail like a closed, angled corner with a short flat at the end. If the control can't find a way to shove the cutter into the corner, it never solves for the intersection points.
 
Are you sure? I've done things like a .139" hole with a .125" cutter, using wear, and a .002" perpendicular lead-in.
Are we brandy sipping, smoking cigars and debating theoretical cases or are we really trying to solve this? :D

From a theoretical standpoint, it might work but, I wouldn't need ever use it that close. I'd establish comp above the part and then drop the Z into the feature. I'd be afraid of some rounding error causing comp to go wonky while buried full-flute deep in a hole.
 
I think your mis understanding the needed parameters to compute the math to achieve comp.

Example :the .550 bore using a .5 end mill.
Using a liner perpedicular lead in from bore center is a numerical value of .275, and you need a numerical value over the tool radius .25, so you have met the condition needed.
I think your misunderstanding needed values.
 
...And if people insist on talking tenths, well, laser optics are fairly accurate. Angstroms or something, I dunno ...
Angstroms... interesting piece of information. Typical HDD platters have to be flat within 15Å or 1.5 nanometers or so in order to maintain the cushion of air the HDD read/write heads float on. Much more and it disrupts that cushion.

Now back to our scheduled banter.
😜
 
I think your mis understanding the needed parameters to compute the math to achieve comp.

Example :the .550 bore using a .5 end mill.
Using a liner perpedicular lead in from bore center is a numerical value of .275, and you need a numerical value over the tool radius .25, so you have met the condition needed.
I think your misunderstanding needed values.
No, I could almost write the algorithm at this point. I'm trying to picture a half inch cutter banging around with 0.050 total clearance or 0.025" radial. Yeah, with wear it would probably work, as long as we weren't compensating over 0.025" which could just be a reground cutter. Too close for me to want to run that, whether it's Wear or Diameter.
 
I don't know. I'd have to draw this out. He said a 0.5" cutter in a 0.550 hole. Not a lot of room to back up and get a run at it (even with Wear). You're right, there are other ways to do it.
Draw it out! It is absolutely correct both geometrically, and in adherence to full dia comp rules.
If your smallest programmable increment is .0001, then a 1/2" endmill needs to be programmed to move no more than .2501 to achieve full ramp distance.

You might be correct on this. All six slides were off the top of my head. I think it may still choke because the cutter never touches the vertical line. CADAM used to gag on that. Dunno about the Haas and that's all I have access to. I'll trust that you've tried it and it worked.

I didn't just try it, I use it all the time.
I don't know what CADAM is, but the vertical line is absolutely "touched", even tho it doesn't actually get cut.
Neither the tool nor the control cares what your finished part should look like, all it cares about is the physical possibility to position the tool where it was programmed to.
Haas and Milltronics accepts it just fine on mills, so does Fanuc and Mitsubishi on lathes, or Fanuc on Wire EDM. ( that's all I have )
Again, if it is possible to calculate the target position, then it is fully compliant with the rules.

I can think of other examples that would fail like a closed, angled corner with a short flat at the end. If the control can't find a way to shove the cutter into the corner, it never solves for the intersection points.

Once again: If the motion cannot be solved, then the control will not try to solve it for you!

Are we brandy sipping, smoking cigars and debating theoretical cases or are we really trying to solve this? :D

From a theoretical standpoint, it might work but, I wouldn't need ever use it that close. I'd establish comp above the part and then drop the Z into the feature. I'd be afraid of some rounding error causing comp to go wonky while buried full-flute deep in a hole.

It isn't theoretical at all!!!
I typically use a standard 4fl. endmill to dial in slip-fit dowel holes that are calling out .001 or more SF!
If it is a 1/4" SF with a +.0015 / +.002 tolerance, it gets drilled ( often without spot ) to something Let B or C, then plunged with the 1/4" endmill and immediately profiled to size with same endmill.
Proper or not for all the purists, I don't give a fuck, It works!
 
I don't know what CADAM is,
PTC owns it or has some "partnership" deal with whoever does now, it's still sold and sort of specializes in ship design. Not just the hull shape but piping, machinery layout, bulkheads, all that stuff. It's kind of cool.


Laughing. 1968.

"The software facilitated the creation of multiple views of an object without the need to use temporary construction lines. Using this methodology, it was possible for a user to design elements such as a pocket with sloping sides and then program a five-axis milling machine to cut the sides of this pocket using an approach called swarf cutting."
 
Last edited:
With this comp talk people will find this similar tech interesting.
I used to run a 3d scanner in the dental lab field, it was used to scan in dental geometry to design crown and bridge and implant substructures.

it actually used a precision sapphire tipped probe that used gravity at just over a 45° angle, physically riding on the stone or titanium model to scan in.

the part rotated around centered on a turn table gathering data points lifting a tenth of a millimeter per revolution, creating a spiral of 3D data points.

to comp the round ball tool to create the model, spheres of the same size were copied onto each data point, and a boolean operation done to subtract the spheres to create the model.
 
THISSSSSSSSSSSSSSSSSSSSSSSSSSSSSSSSSSSSSSS!!!!!!!!!!!!!!!!!!!!!!!
no reason it shouldnt be able to put in a wear setting vs dia/rad
It looks like at least the recent Renishaw macros do have an option to set for doing wear instead of diameter.

Macro 9852

Scan through the program until you find:
#2=#4 (CHANGE TO #4 FOR DIAMETER)

Change that to:
#2=#19 (CHANGE TO #4 FOR DIAMETER)

So #4 becomes #19 and it changes to recording wear. I just confirmed this on my 2004-2005 Inspection plus software and it's in there all the way back then.

Thanks to this video:
 
It looks like at least the recent Renishaw macros do have an option to set for doing wear instead of diameter.

Macro 9852

Scan through the program until you find:
#2=#4 (CHANGE TO #4 FOR DIAMETER)

Change that to:
#2=#19 (CHANGE TO #4 FOR DIAMETER)

So #4 becomes #19 and it changes to recording wear. I just confirmed this on my 2004-2005 Inspection plus software and it's in there all the way back then.

Thanks to this video:
"Even a blind squirrel finds a nut" :D
 
I just program in my
We haven't had a good fight around here since EmGo told us that he won't use lathe canned cycles. It's time for another and probably a whole lot more controversial: cutter comp, CAM and offset methods.

I bought a Haas VF-2 in 2004. It was ordered with Renishaw probing and tool setting. The Renishaw software records tool offsets as actual length from the spindle gauge line to the tip of the tool, positive length. The diameter of the tools is recorded as the actual diameter, as calibrated to a measured gauge pin. This method has remained consistent through all the Haas I've used since that time, and includes the current day machines. Tools often measure about 0.001" undersize which is probably right.

Since the Renishaw software is somewhat standard, I am assuming this method of measuring and storing tool lengths is consistent across machines that have Renishaw software installed.

If I program to use cutter compensation in Mastercam, select Control Comp and go. Make sure the cutter diameter is smaller than any lead-in, lead-out moves and fits in all the corners and it's good. Seems like that's part of selecting the proper cutter anyway.

For years, I've heard old timers arguing to zero the diameter values and do everything using the Wear offset method (and matching that selection on the CAM side, of course). I fully understand how it works and I still can't come up with a single reason why anyone with an installed presetter should use that method, or wants to use that method.

Fast forward to yesterday: one colleague sold his Haas to another. Move is complete. A couple of guys in the new shop have done some very basic running of CNC but, zero programming. They know the basics of offsets and how to run the Mastercam code supplied by an outside programmer. He sends setup sheets with a tool list, origin and holding details. They want to learn how to use their machine and will soon go to Mastercam and Haas training. I've done hours of training with them at the control, including how to install and preset a tool using the Renishaw OTS. Their contract programmer does this full time and obviously knows his way around Mastercam.

I take a part that was originally programmed for their Centroid-equipped Bridgeport. Codes all look compatible so we run it on the Haas in Graphics mode. It appears to run fine, gets to some lead in moves and blows up. Okay, he used wear. I try to explain this to the new guys. Hey, call or text your guy. Tell him you're on a Haas now. You have Renishaw probing. It records actual diameters, not Wear. You need him to change Comp to Control and repost it for you. I assumed that was as pinpoint specific as it could get. A reasonable guy would have realized where they are and done it.

Instead, after multiple back and forths, we get nothing but arguing about how they shouldn't be using Diameter and should do everything as Wear. From the exact wording of the messages, I've made it abundantly clear that I know Mastercam and know exactly what I'm asking for. He never gives us what was asked for. Fine. I subtracted out the diameters to get net wear values and ran the job.

I'm training. I'm trying to show these guys how their machine works. The programming guy should be trying to help his customer get the best part they can and help them along the journey of using this stuff. If the customer is using Renishaw Inspection Plus routines and they record diameter, it's his job to give them what's most compatible and least likely to have an error with new users.

It got so bad that while we were waiting, I was telling them exactly what his responses were going to be and it didn't fail. He refuses to supply Diameter (control) comp output. We got through these parts. I showed them how they can preset the tools and then subtract out the nominal diameter to arrive at a wear value. They can do it differently later if they like.

And now to the question: I'm an open minded guy. It seems to me that if Wear offsets were truly the way to do things, Renishaw would have changed the method of recording diameters somewhere in the past 20-25 years. Who uses wear offsets with a pre setter and why?

View attachment 437975
I just set my tool, and measure it's diameter on the tool-setter in my haas.
Oh, it says 4.9963" Ok, I'll program with my trusty 4.9963" end mill.
All else is for the birds. I am too busy to split hairs.
 








 
Back
Top