What is your customary way to set tool offsets for your CNC Milling Machine?
Do you enter the diameter of your tool in the actual diameter column?
Probing if available, if not, paper…
I teach my students to do all 4 ways. They may go to work for a shop that does not have probing. I have found an issue using the probe and having it measure the OD of the tool also. When it puts in the actual diameter, if my lead in and lead out default I usually get an error when I run the program in the machine.
The students check their program in a simulator before going to the floor and the error did not pop up. Of course the simulator the actual diameters were zero. Sooo, the question, is it normal practice to leave the actual diameters at zero, or do you measure the diameter of the tool with probe?
Depends on how big of a shop your in. Small shops get buy with a feeler gauge or a 1-2-3 block , medium size shops usually use a Renshaw probe, big shops with a lot of money in equipment / personnel will have a tool setter and a tool crib person who will get the tool in the holder +/- .01 , dynamic balance it for high rpm operations and give you the tool length, so you just need to load the tools. It’s surprisingly easy to store tool lengths in programs
I learned the old fashioned way… paper.
A machinist should know all 4 ways. But because my machine has wireless probing, I use that most of the time.
Personally I would stay away from measuring with number 3. Because I have seen too many people make mistakes by forgetting to offset the gauge block or HSS blank distance. This usually results in scrap.
But if you don’t have distractions, like co-workers then you can do it.
Know it all, use what is best for current situation.
Sliding head mill/turn all set with paper.
I think people should know all of the ways to touch off a tool. Tool probes are great but at some point you will need to know the manual way to do it. Definitely prefer gauge block over paper as it is more accurate.
I also believe it is safer and better practice to use actual tool length. Have seen a lot of people who have a large negative value for their tool length (from machine home to top of part face) and I have seen it bite people. A huge negative is too hard to tell if the length offset is correct or not at a quick glance.
If you are using cutter comp in tight spaces I think it’s much easier to use wear comp and leave the tool diameter at zero. This allows you to have a small move to turn comp on and off instead of needing a larger motion based on the actual tool diameter in the geometry register.
We use the edge technology pro touch off gauge. Makes it real easy to check tool height with no real chance to break the tip of endmills.
Gauge block from a common area on the table with a ground dowl pin to roll under the tool tip. This makes sure everything is coming off one common point that can be repeated over and over again.
If a tool breaks it’s easy to resett it and have it perfectly set to the other tools again. Ever try resetting a tool height from the top of a part that has already had its surfaces machined? Just not good practice.
We will then use paper to find the top of the part and subtract the two points to enter into the WCS z offset. All of our parts are programmed from the top of stock so It’s pretty easy from there.
We do not have probing, So I can’t comment there. I can see one of those spring loaded ones like the Edge Technogy could probably be a bit faster Than using the gauge block and pin technique. We may try one out, as it’s not too expensive - and we are rebooting our processes in the shop.
NOTE we really don’t care that the tool tip is a perfect 2" or whatever above the table or the part, just as long as it’s a repeatable height that we can get a tool to quickly.
That’s a pretty nifty tool and its fairly cheap. I am going to try to get my hands on one of them.
For the diameter, it depends on how you program.
Like “in control”, “wear”, “computer”.
I use wear and have the tool diameter column blank.
If i have a tool cutting a 1 inch square and it comes
out to 0.998, I put a positive 0.002 in the diameter column to get the 1 inch.
And for touching off, just like what Donald_Rockey suggested,
I use one of these for consistency since i dont have probing on my machine
I touch off with a a piece of fritos bag.
I use cutter comp in the wear column, not the actual diameter.
@Titan in one of his training videos has great strategy for using a gage block or spacer to set tools… We made a 3/4" diameter with a 1/4" hole x .2500" thick spacer. Ground to thickness and hardened. Just like Titan they touch off each tool with spacer and then when completed, subtract the .250 from every tool height offset at the end as one process. Yes, they have to do this uninterrupted, but it can be done quickly. They bring the tool below the gage block and then slowly increment up in Z until the gage block slides under it, they one click down and change increments to .0001" and one click up until the gage block again slides under it. I used to have students break inserts using the paper method.
@StephenHadwin this works great until you have a worn machine and people that don’t know how to check and adjust backlash… 
The “one click down” should be .005-.010 increment to make sure coming back up gives room for the backlash and still have room to move in .0001’s to get to your true set
The best way that I have found on fanuc controls is to write a tool change program with an m00 between each tool change so you can bring the head down with tool and touch off of the base rails of the vise. I use a .500 dowel pin the I put a -.500 offset in the Z G54-G59 for the compensation of the dowel pin so you don’t have to add .500 to each tool when you touch off. if you zero the relative z at z machine home position on fanuc controls you can bring tool down and hit input calc soft key and it will automatically put in the z value. (on fanuc 10-11 controls you have to pick which axis) Once I hit input calc I immediatally arrow down to the next tool and put in auto to cycle start next tool cnage and repeat process. once you have all of the tools touched off of the vise base rails you can put a positive value for your parallel height and finished part height in the G53(common) to offset for the part and parrellels. if you are using multiple offsets though you will have to input + into each individual offset the height difference from your -.500 to have multiple height fixure offsets but that doesn’t happen that very often. I’ve notice that using a round dowel pin is easier than using a guage block as for it is easier to slide under the tools without damaging flutes on smaller endmills and carbide drills and indexable cutters. If you are using a haas or a fadal they have automatic tool setting features so you don’t have to do the process like I do have to on a Fanuc control.
Chris that’s a very interesting concept setting the z off the bottom of the vice working your way up. I’ll have to consider that. I like the idea of using a dowel pin because they are inexpensive and rather disposable compared to a gage block or 1 2 3 block.
You could even further automate that process by writing a macaro once you have your tool height that automatically detects which tool is in the spindol , fills in the appropriate tool length and tool changes to the next tool.
I also used a .020 plastic shim stock to make all of my tool sets on small & very large lathes.
At work, all our milling machines have both a tool probe & part probe.
Fist the machine would calibrate the part probe using the tool probe, since the part probe was more sensitive to movement then the part probe, then the part probe would probe the part to locate the part of where is was in relation to the machine.
I do have to make disclaimer that we used fixtures for every part & every operation so the part probe ($5,000 to $15,000part probes) was in no danger of crashing into the part. The only reasons that our part probes cost so much is because who made them and how many contact points they had. I had seen 5 part probes being crashed into parts and rendered useless because of simple part & machine control software errors on just one machine engineering & maintenance were trying to get set up.
Then the machine would probe every tool so the machine would know if it was the correct tool & within tolerances.
A good part & tool probe should only about $5,000, but using a .020 shim plastic stock would work just as well for most tool sets.
well, i use the plastic film from the cigarette pack
It works 100%