What's new
What's new

Renishaw and the cutter diameter conundrum: the offsets holy war

Donkey Hotey

Titanium
Joined
Dec 22, 2007
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?

Crowder.jpg
 
I searched and couldn't find anything last night.

FWIW: if you're doing presetting manually and you run your own code, you do you. Whatever turns your crank.

On the Haas, chip load and SFM are shown based on data in the table. I also can't tell which tool is the 1/2" from looking. It's anyone's guess. The diameters are all zero or close to it. Worthless.
 
When I program, I use comp in the computer and comp in the control. I've never measured diameters on my tool presetter.
The code already comps for the tool diameter so I use wear to tweak final sizes if I need to.

No particular reason. That's the way it was done when I first started on CNC mills so I guess it's just what I'm comfortable with.
 
I searched and couldn't find anything last night.

FWIW: if you're doing presetting manually and you run your own code, you do you. Whatever turns your crank.

On the Haas, chip load and SFM are shown based on data in the table. I also can't tell which tool is the 1/2" from looking. It's anyone's guess. The diameters are all zero or close to it. Worthless.

You will probably need to google it, the search function here is garbage and it was probably a completely unrelated thread that went off on a tangent and then everyone got excited.

I have both - manually preset tools and auto set tools, varies by machine. Wear comp only regardless.

I wrote a bunch of reasons in that other post (and god knows how many others before it), but really they all boil down to one fundamental thing - diameter comp creates a hard disconnect between the cam simulation and reality.
 
I wrote a bunch of reasons in that other post (and god knows how many others before it), but really they all boil down to one fundamental thing - diameter comp creates a hard disconnect between the cam simulation and reality.
I get what you're saying because--yes--if someone loads a 2" cutter where a 0.25" was expected, the path will be completely different.

If Wear were "the right way", there could be a single Macro value set during calibration that could have turned all output values became wear. Example: Tool Length and Diameter already prompts for approximate dimensions. If I entered 0.25" before setting, it would be easy enough to subtract that from the result before recording and put it in the wear column.

Renishaw has never bothered to do this (to my knowledge). Any arguments contrary to this simply suggest that all of Renishaw and 20+ years of history are and were wrong.
 
One thing to mention you say the probing puts in the diameters in and you zero them out, there are routines for just probing for length without any diameters.
I would agree with others that adding in the functionality of having diameter numbers in the control is just another place to add user error for no benefit.

but we have already had this entire argument before.
 
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'm glad you brought this up, i was literally about to start a thread about this topic.

for the same reason as you, i have my defaults in NX set to output 'in control' compensation = you need to have a radius value in the tool diameter page.
its bitten me a few times where i had to revert to 'wear' and take the diameter out of the offset page because certain toolpaths were giving me errors using 'in control' comp, which led to fucking up a few very expensive parts. of course - my fault, i should have slowed down and double checked.
but i'd really like to try to understand why fucking wear comp causes so many goddamn issues with every cam system i've used, and with every control i've used. always something making it unhappy!

the issue now is that if i go back to using 'wear', i cant probe my tools because the cycles require a value in the diameter offset. so either i have to fuck with putting in a radius before measuring a tool, then going back to zero, or keep using in control comp, and deal with potentially fucking shit up if i need to switch to wear on some toolpaths...

can you tell i'm f'kn pissed?
 
One thing to mention you say the probing puts in the diameters in and you zero them out, there are routines for just probing for length without any diameters.
I would agree with others that adding in the functionality of having diameter numbers in the control is just another place to add user error for no benefit.

I've used diameters exclusively for 20 years now. Not only never had an issue but, it eliminates errors.

Then again: you're a guy who breaks down every setup. I keep tools in the same pockets, with the same offsets forever. That way I have a library of tools I can pull into a new Mastercam file, be programming in 2 minutes and go straight to the machine with the output. The 1/2" endmill is where it always is, it matches in the table and if it wears out, I can touch off a brand new one quickly. Anyone else walking up to the machine can scan the offset table and see where the 1/2" end mill is.
 
i'm glad you brought this up, i was literally about to start a thread about this topic.

for the same reason as you, i have my defaults in NX set to output 'in control' compensation = you need to have a radius value in the tool diameter page.
its bitten me a few times where i had to revert to 'wear' and take the diameter out of the offset page because certain toolpaths were giving me errors using 'in control' comp, which led to fucking up a few very expensive parts. of course - my fault, i should have slowed down and double checked.
but i'd really like to try to understand why fucking wear comp causes so many goddamn issues with every cam system i've used, and with every control i've used. always something making it unhappy!

the issue now is that if i go back to using 'wear', i cant probe my tools because the cycles require a value in the diameter offset. so either i have to fuck with putting in a radius before measuring a tool, then going back to zero, or keep using in control comp, and deal with potentially fucking shit up if i need to switch to wear on some toolpaths...

can you tell i'm f'kn pissed?
Your probing doesnt have cycles for length only? strange? So it has diameter for drills also?
 
I've used diameters exclusively for 20 years now. Not only never had an issue but, it eliminates errors.

Then again: you're a guy who breaks down every setup. I keep tools in the same pockets, with the same offsets forever. That way I have a library of tools I can pull into a new Mastercam file, be programming in 2 minutes and go straight to the machine with the output. The 1/2" endmill is where it always is, it matches in the table and if it wears out, I can touch off a brand new one quickly. Anyone else walking up to the machine can scan the offset table and see where the 1/2" end mill is.
Still, the last time we went through this, the control comp with dia. guys lost (you :D) , CAM comp with wear is where most said is a less error system, sorry brotha!! The I's have it:D
 
the issue now is that if i go back to using 'wear', i cant probe my tools because the cycles require a value in the diameter offset. so either i have to fuck with putting in a radius before measuring a tool, then going back to zero, or keep using in control comp, and deal with potentially fucking shit up if i need to switch to wear on some toolpaths...

can you tell i'm f'kn pissed?
For these guys, after enough back & forth and watching me, I showed them how to pull out the nominal diameter. As most of us are aware on Haas: they can do the Renishaw thing, get a true diameter of the cutter, then go to that field on the offset table, -0.5" and Write/Enter to subtract the nominal out of the measured value. Instant negative "wear" number.

It works. I guess. The silver lining was that this showed them how to do math in their offset table. I was deliberately trying to not overwhelm them and would rather not have had to do that yesterday. They handled it fine.

It dovetailed nicely into me adding 3" to the G54 Z value and dry running the part above the vise. Showed them how they could stop the machine, go in with a 123 block and see how deep each cut will be. Check vise clearances. Take out the 3" when they're done and ready to run for real.

It was a positive day but, didn't want to get into this smoking lounge, brandy sipping debate while they're trying to learn what G54 is.
 
Still, the last time we went through this, the control comp with dia. guys lost (you :D) , CAM comp with wear is where most said is a less error system, sorry brotha!! The I's have it:D
Maybe you think the Wear guys 'won' (whatever that means in this field--all of these arguments have merit for different needs). I'm still arguing that if Control comp sucked so badly, Renishaw would have responded to changing or at least making it an option by now and they haven't.
 
Maybe you think the Wear guys 'won' (whatever that means in this field--all of these arguments have merit for different needs). I'm still arguing that if Control comp sucked so badly, Renishaw would have responded to changing or at least making it an option by now and they haven't.
I don't know what you mean, they have tool probing for what ever system you want, not sure what your wanting them to change?
 
i'm glad you brought this up, i was literally about to start a thread about this topic.

for the same reason as you, i have my defaults in NX set to output 'in control' compensation = you need to have a radius value in the tool diameter page.
its bitten me a few times where i had to revert to 'wear' and take the diameter out of the offset page because certain toolpaths were giving me errors using 'in control' comp, which led to fucking up a few very expensive parts. of course - my fault, i should have slowed down and double checked.
but i'd really like to try to understand why fucking wear comp causes so many goddamn issues with every cam system i've used, and with every control i've used. always something making it unhappy!

the issue now is that if i go back to using 'wear', i cant probe my tools because the cycles require a value in the diameter offset. so either i have to fuck with putting in a radius before measuring a tool, then going back to zero, or keep using in control comp, and deal with potentially fucking shit up if i need to switch to wear on some toolpaths...

can you tell i'm f'kn pissed?
Which control is this? Heidenhain?

I don't think I've ever used a control/measuring cycle that forced me to enter a diameter...

My only heidenhain is a lathe...
 
I don't know what you mean, they have tool probing for what ever system you want, not sure what your wanting them to change?
As an example: during installation and calibration of the OTS, it asks for a number to tell it which side of the table it's located on. It uses that variable forevermore to know where the OTS is pointed so it doesn't clank into it. It also asks and records the pocket for the probe (I know we all know this--stating it so we're on the same page).

It would be child's play to ask for one more macro input for whether you want to use Radius, Diameter or Wear for measurement methods.

Once set, all other macros could subtract, divide by two or whatever you wanted, to record where and how the value gets stored. The tool routines already ask for the nominal dimension. Everything is there to do it.

If someone were so bothered by Diameter, they could take the time to rewrite the Renishaw routines to do this for them. Again: if Diameter is wrong, why haven't they done it?
 
Yeah I guess if I had to use a Haas and pre-enter diameters so that it will offset the tool cutting edge to be measured properly, then I would just go to the diameter column, origin, column.

edit: I am guessing it is because they do need a starting value to be able to offset the tool over so the cutting edge hits the center of the probe, but then after that, you either leave it and use it, or zero the column out, pretty simple.
 
Yeah I guess if I had to use a Haas and pre-enter diameters so that it will offset the tool cutting edge to be measured properly, then I would just go to the diameter column, origin, column.
My understanding is the Renishaw Inspection Plus macros are common across compatible (Fanuc?) controls. No?

Auto Length Only: works on drills, pointed tools and tools small enough to contact the anvil. Doesn't need a diameter or length and doesn't do anything to the diameter or wear fields.

Auto Length and Diameter Rotating: needs approximate tool length and nominal diameter so it knows where the tool tip is for getting it over the center of the anvil. Already knows the diameter because I just typed it. Easy enough for the macro to subtract that out.
 
i'm glad you brought this up, i was literally about to start a thread about this topic.

for the same reason as you, i have my defaults in NX set to output 'in control' compensation = you need to have a radius value in the tool diameter page.
its bitten me a few times where i had to revert to 'wear' and take the diameter out of the offset page because certain toolpaths were giving me errors using 'in control' comp, which led to fucking up a few very expensive parts. of course - my fault, i should have slowed down and double checked.
but i'd really like to try to understand why fucking wear comp causes so many goddamn issues with every cam system i've used, and with every control i've used. always something making it unhappy!

the issue now is that if i go back to using 'wear', i cant probe my tools because the cycles require a value in the diameter offset. so either i have to fuck with putting in a radius before measuring a tool, then going back to zero, or keep using in control comp, and deal with potentially fucking shit up if i need to switch to wear on some toolpaths...

can you tell i'm f'kn pissed?
Like empower, but machining injection molds you don't really need or use any comp, why because you rendered it on the computer, and it was fine after many many hours of watching a rendering.
I don't then want to go put it in the machine, and let it comp it and fuck it up and ruin a very time consuming expensive part, loosing weeks of time and money.

So I don't use any comp at all for injection molds, but back in Nam when I tried (control dia comp) because that's how we made parts, it fucked up a couple too many times, so that was the end of that.
 
My understanding is the Renishaw Inspection Plus macros are common across compatible (Fanuc?) controls. No?

Auto Length Only: works on drills, pointed tools and tools small enough to contact the anvil. Doesn't need a diameter or length and doesn't do anything to the diameter or wear fields.

Auto Length and Diameter Rotating: needs approximate tool length and nominal diameter so it knows where the tool tip is for getting it over the center of the anvil. Already knows the diameter because I just typed it. Easy enough for the macro to subtract that out.
Agree, they should add an option to keep or subtract that out, it is a click away to zero a column so maybe that's why they don't. Who knows.
 








 
Back
Top