Tool wear explanation and suggestions

[marc7X3XJ]

I have searched the forum and found a little info here and there but I am still a little fuzzy on the subject of tool wear and compensation. None of the explanations that I have found make total sense to me and I do not want to jumble together random tidbits of information and end up with a disaster on my hands.

I am currently using my nominal tool diameter from my tool library and leaving the compensation set to in computer. On a few operations I will then go back to the CAM and adjust the Stock to leave in order to get within my tolerance where it is critical. This is ok but then I need to output new code when I replace a tool and can not make quick adjustments at the machine. I have been working this way in my shop for almost 20 years but I would like to learn how to effectively use the tool wear feature as I move more into production parts to improve standardization from batch to batch.

Here is where I get fuzzy. I believe that I need to turn on the "In Control" cutter comp or "Wear" comp and I am not sure which is best used in different scenarios. I have a few simple questions and I am open to suggestions from those with more experience.

1. I use my Renishaw to calculate the length and diameter of all cutters other than drill and chamfers on my Haas VF2SS. This auto populates the "Length Geometry" and "Diameter Geometry" columns. Is there a way for the system to calculate the difference between the assigned "Diameter Geometry" and the entered "Approximate Diameter" to the tool "Diameter Wear" column? Am I wrong in thinking that this would be the proper dimension entered in the tool wear column?
2. If I choose the "In Control" compensation option will the program run based on the size that is detected by the probe and assigned to the "Diameter Geometry" column for an accurate part dimension?
3. If I post code using the "Wear" compensation based on my nominal tool diameter in my tool library and the total between the "Diameter Geometry" column and the "Diameter Wear" column are equal to the nominal diameter will that give me an accurate cut?
4. What comp is best used when and what offset columns are applicable to each of the comp selections?

I am pretty sure that I am overthinking this and it is probably simpler than I am making it out to be but I am definitely confused by what columns are utilized with what commands in each scenario.

[seth.madore]

If your machine accepts cutter comp, I strongly encourage the use of that on all finish passes. Roughing passes, imo, do just fine with Computer Comp and "Stock to Leave" set appropriately.

As for which one to use (Control or Wear), it all depends on personal preference. In my own shop, I use "Wear" on every mill program. Why "wear"? With Control Compensation, you're required to input the full radius or diameter of the tool. In the years before I had a tool setter on both machines, tool offsets were all input manually, both length and diameter. Switching to "Wear" compensation only required me to input lengths, as the "Wear" value should be zero. Having one less thing to worry about was just common sense as far as I was concerned.

I have a Renishaw OTS system on both my machines. To touch off tools and input a value to account for a change in tool diameter (off of nominal), I have to input what's called an "Experience Value". This is what the theoretical radial value should be. Example:

G65 P9857 B3. D.5 J.25

This would command a length and diameter setting for a .500" tool, assuming of course that your machine wants to see radial values. (I may be mistaken on that bit, Haas and Fanuc can handle either radial or diametrical offset values I think) 

Personally, if I'm running Wear Comp, I still just establish length of tool and not bother with diameter check. If my tool has worn to the point where I'm not going to make a close to perfect part right off the bat, it gets tossed right in the scrap carbide bucket. That's not to say I'm wasteful, but if I have to comp out more than .001" or so, it's likely past the point where most of my work will tolerate, both in finish and accuracy.

[marc7X3XJ]

'I guess that I am not looking to use the "Wear Diameter" so much for actual wear but to dial in the new tools that are rarely the actual nominal diameter. Most are between a few 10th off to a 1000th or so with a few larger tools. For instance if I put in a new 1/2 end mill and then Renishaw tells me that the "Diameter Geometry" is actually .4989 then I want my machine to offset the tool  for the other .0011" diameter(.00055" radius) so that my finished part is the proper dimension and not undersized in pockets and oversized on profiles when I post the code using a .500" nominal tool diameter. I hope that I explained that right. I do not use heavily worn tools. It is not worth the problems that they cause.

Marc

[Ketherton21]

you should have your tools in fusion taught as the actual diameter of the tool you are using. 

or if you dont want to use the wear, use negative stock to leave (assuming the tools are undersized/regrinds or whatnot)

wear is the best to use and what everyone i have ever worked with uses and from my experience industry standard almost most programmers always use. saves trips to the computer, which is good if its in another building or even 5 feet away. but i think to use "wear" you actuyally use "in control" and you can just add your radial values into your finish tools.

if you are using the same tool to rough and finish use "setup, manual NC, force tool change" that way you can just T up or T down to your finish pass alone and re run it after setting a wear value.

youll know when you have the right thing selected because it will generate a D value in addition to H value. the D value typically is the same as your tool number but you could theoretically make it any number you want. which can get confusing thats why some people just add 50 or something. so you could have t0101 H1 D1 or T0101 D51

additional id like to add I hate regrinds unless its 1 time grinds.

[marc7X3XJ]

I understand the advantages of using "wear" I just do not know how to do it. I understand that I select it in Fusion but what does that actually do and what dimensions need to be applied to the tool offset table. Do I need the "Diameter Geometry" column filled out with the nominal tool size or is that output from Fusion? Do I leave the "Diameter Geometry" column blank? Do I enter the difference between the nominal tool diameter and the actual tool diameter in the "Wear Diameter" column? Do I enter the actual tool diameter in the "Wear Diameter" column? The are a lot of potential options and I have yet to see a simple explanation of what to enter where based on "In Control" or "Wear" selection.

[Ketherton21]

when you set tools with your probe is it pulling the diameter into the diameter (D) column? 1 column to the right of that. the (wear D) column, your values will be small like .001, .002 or negative (this dimension is radial and incrementally added to the tools existing dimension)

if you bore a 1.000" hole, and you have finish with a hole that is .999" , set your tool wear D to  -.0005

think of your WEAR D, as the same exact thing as "leave stock"

[marc7X3XJ]

So basically the total between the "Diameter Geometry" column assigned by Renishaw and the "Wear Diameter" column should be set to equal the nominal tool diameter used in Fusion?

[Ketherton21]

in a sense. adding the wear is how youd compensate on the fly from part to part to account for tool spring or wear. if you are only doing 1 part I wouldnt even worry about the wear, just make your tool in fusion the diameter your probe is telling you it is.

also you might want to check your probe and calibrate it. if the carbide has ever been replaced on it its probably not the same. thats getting into an entire other can of worms tho. and ive never had to change my macros on the mill only the lathe. Haas was just here and said they can vary by up to .08"

[Anonymous · Accepted solution]

Wear offset is used to correct for tool wear, you start with fresh cutting tool and assuming it cuts on desired path, value in wear offset register should be zero.

Now, as you make parts, tool starts to wear on cutting edges of end mill or turning insert.

That tool wear results in change of size on machined part and you use wear offset to correct for it and keep the size constant.

When you use in computer compensation, all compensation is calculated in computer, there is no need to add tool radius or diameter into machine control tool offset page.

On top of that, using wear compensation for finish pass in Fusion simply means you start with zero in tool wear offset and if the initial part is off desired size, you can use small value in wear offset to dial in for targeted size as well as correct for tool wear down the line.

To recap.....

If you are using in computer compensation for roughing, you should clear any data from diameter or radius register in tool geometry page of your machine because all compensation is already included in resulting G code.

If you use wear compensation in finish pass, start with wear register at zero.

Instead of leaving (or adding) stock and regenerating tool path, use wear offset to correct for size.

The reason why you want to clear diameter or radius register is because using wear compensation in finish pass will result in G41 or G42 being generated in g-code.

If you have any value in D or R registers, it will be considered when G41 / G42 is activated and it will result in double compensation.

[marc7X3XJ]

That is the part that I was missing. I need to clear the Renishaw assigned diameters if I want to use the Wear compensation and that small adjustment only applies to finish passes.

Now the next part of my question would be that if Renishaw tells me that my new tool is .499" and not the nominal .500" that the tool should be then would it be ok to add .001" (or -.001")to the Wear column when I delete the Diameter Data?

I have been thinking that tools are cut undersized as an acceptable tolerance but now I am wondering if it is not intentional by the manufacturer.

Thank you,
Marc

[marc7X3XJ]

It is a new machine and Haas was just here setting it up a couple weeks ago. The probe was setup within a tenth or two when we did it so that should not be an issue.

[Ketherton21]

Wear is radial, you want to go half.

Or leave it at 0 and instead change your tools dimension in fusion itself to .499

in this case I wouldn’t worry about the wear unless you are doing multiple parts. 

if you want fusion to keep .5 as tool diameter then enable wear and add -.0005 to your WEAR D value. 

or add -.0005 stock to leave in fusion. 

[marc7X3XJ]

Changing stock to leave is how I have been doing it for years and it is fine for a few parts but I will be doing larger runs of some new products and do not want to generate new code every time I need to replace a tool. I would rather post with the nominal diameter and then make fine adjustments in the Wear column as needed at the machine.

Thanks again,
Marc

[seth.madore]

Changing Stock to Leave in Fusion to account for tool deflection and size variation should really only be done if your control doesn't allow for compensation, such as on the older Tormach controls. Once you start using Wear and become comfortable with the process, you'll be glad you did

[Ketherton21]

3000000% agree. its pretty impossible to convince people who are stuck in their ways though (not referring to anyone here) we can try tho right?