How to Use Cutter Comp on a Tormach! WW180

Cutter Comp in Fusion 360. Let's explore Cutter Comp by "walking-out" the diameter of an interpolation bore! Force-feeding information to CNC controllers is the norm and while it might sound like it's not a big deal, Cutter Comp is a Fusion 360 nuance that packs a punch. Cutter Comp allows us to easily update tool diameters, maintain tolerances, and improve work-flow. It works well for "walking-out" bores but there's an even BETTER application for it yet...Threadmilling.
NYC CNC Publishes weekly content on CNC, CAD, CAM & Manufacturing including the Wednesday Widget CNC project and Fusion Friday Fusion 360 tutorial! 5 Reasons to Use a Fixture Plate on Your CNC Machine: bit.ly/3sNA4uH

[@gredangeo]

I prefer to use "Wear" offsets, not "In Control" That way all your code is based from the center of the tool as normal. The key reason for this method is because in the Controller, all your offsets still say "0". You don't have to keep track of the tool diameter. (Accident waiting to happen). In your example John, you were going from .1875" to .1873". If you were using "Wear", you would put in -.0002". It's better to think about the toolpath as: 'Say, I want to push the wall further away from where it is. How far do I want to go? 'Negative Two Tenths'. *A negative value will remove material* Is a great way to remember it.

[@EdgePrecision]

John, to avoid cutter comp errors in a compensated tool path all lines and arcs in the compensated path have to be able to touch tangent to the radius of the compensated value. Or to say that a different way no inside radius can be smaller than the compensated radius. And no lines can be so short that the tools radius won’t touch them. In your circle/bore you can mill it with a tool just slightly smaller than the size if these conditions exist. Let’s say you force you cam software to enter at the holes center you could easily use a tool of .375 diameter by making your lead in line say G41 X.190; G03 X-.25 I-.22; G03 I.25; G03 X.190 I.22; G40 G1 X0; That’s with your zero at the hole center climb milling a.500 diameter.

[@jimhimesjr]

Edge Precision exactly. This is why I always preferred wear comp just comping a small amount. Has all the features of cutter comp without the large comp moves needed. Hand coding is where I always thought control comp was best. It is nice for following the program/part print and diagnosing errors though.

[@jasontartaglia5864]

Absolutely wonderful video describing cutter comp

[@stevewylie5086]

Great vid John. On my homemade setup I carefully measure the tools carbide are more often a lot smaller than nominal and putting that in the tool library in fusion works for me.

[@lesstrickland6891]

Awesome vid. This was actually the next thing I wanted to learn. I was getting tired of having to force it with "Stock to leave". Thanks!

[@hdfanboy]

I couldn’t imagine not running any milling ops without cutter comp where I work. Maybe for job shop work where it’s one off or very short runs but when your running hundreds of parts and you might have to make minor adjustments every now and again it makes a massive amount easier using cutter comp.

[@danm3071]

Same with our Shop. It helps the operators see the exact position as it matches the print and then adjust wear within cutter comp screen.

[@hdfanboy]

Yep absolutely right. It would look weird having a random number in the program and then the operator wondering where this number came from.

[@chriswilson746]

Use Wear v.s In machine, a standard cam (In computer) tool path only posts a g43 line for in control length offset. i.e fusion is doing the radial side comp and the control is handling the length offset. If you use wear compensation, then fusion still does the radial/side comp but the code now added a g41/g42 so the control is being told to do length and side compensation even tho fusion did a the radial/side comp... this means the value in the dia offset is just the difference from spec v.s actual. i.e All tool paths can be marked as wear and as long as the dia is zero on the offset page for the given tool, the code runs the same as standard. but if you need to walk a tolerance in then you just add a small neg value in the dia field like -.001mm then the controller offsets the tool path...Think of it as a fine adjustment or stacked compensation fusion does 99% of the compensation and the wear/dia value is the controller offsetting the tool path for a final tweak. great for tool deflection or even material change or tool wear etc.

[@OakwoodMachineWorks]

YES! THANK YOU JOHN!

[@TheDestroyer1250]

I've worked in shops where CAM software was frowned upon and or they didn't want to buy licenses to Mastercam or other brands of software. I would have to program complex parts and fixturing by hand and probably wouldn't have any hair left if cutter comp didn't exist. I love Fusion 360 and I use CAM software in my personal shop but I also believe everyone getting involved in CNC should have to do a fair amount of hand programming simply because it teaches the fundamentals of G-code. Another issue is post processing code with older controllers that tend to be very picky on format and code compatibility. Unless you take the time out to edit your post processors and tailor them to various versions of controls, It's sometimes just as quick and easy to add in hand written code or edit code to perform tasks.

[@sp1nrx]

Hand coding for *most* simple jobs is faster than running everything through a system to get code, particularly if there is no CAD drawing to start with. Cutter comp is a necessary part of CNC. How anyone can NOT use it is crazy.

[@LizakDominik1988]

You can avoid that error message by using wear comp. That's how I get around it🖒 Great video 🍻

[@donaldparker4277]

I love cutter comp. Now days I rarely have an end mill that cuts to size. I think the niagara end mills for aluminum are the only end mills I haven't had to use comp on.

[@JohnSmith-iz8wg]

This is a good strategy because a well trained operator can make corrections during a production to ensure that everything stays in tolerance. It might be a good idea to start a new hole after an adjustment to prevent rubbing.

[@adamcain4603]

I always use cutter comp I change a lot of the tools that the programmer picked and we get all are end mills reground.

[@davidl9410]

I got taught how to hand program 2 years before I even touched cam software. Now I can hand program parts quicker then the machine can beep when I press the buttons. and I always use cutter comp as much as possible

[@yandriarce2439]

You can make it even easier by eliminating the drilling operation and open the holes up with a circular ramping cut using the end mill

[@CR3DT]

Great vide that I found by accident. I read many of you are recommending WEAR COMP. How does that work with PP, do you have to manually edit the code at the controller and reload it?

[@bgehret3141]

I like to keep the cutter comp setting "in computer" and then use a cutter comp setting in the controller of the amount by which I want the hole to grow or shrink, e.g. 0.001" or -0.0015.

[@dylanrink3130]

I use fusion and use the in computer comp, when I want to walk in a part, on my Mitsubishi control I just add wear offset of positive number on radius like .0005 no need for actual diameter. negative -.0005 Will take a thou off a holes diameter

[@sp1nrx]

Does the Tormach accept a negative number for the tool comp? On Fanuc with your milled hole a negative number would get a "post" where the mill used the path on the other side.

[@chrisdemchalk3491]

Dumb question- after doing the adjustment for this project would you then leave the updated tool diameter value in pathpilot or revert back to the nominal 3/16 diameter for some next job and perform the walk out if needed?

[@TeslaAtoms]

John, if you re-run the same hole with another diameter in the software, how do you know how much of a difference is from tool deflection when the first pass was taking a real chip and the second was only kind of a spring pass?

[@ikbendusan]

can't you set a pre drill location and use a 2d adaptive instead?

[@mobo9391]

so i have tried this over and over and all I get is a error. arc move in corner can not be reached with tool without gouging. I cant figure out what the issues is???? I even made the tool 4 " long and the cut is only 1/2 deep..

[@JBCreations2650]

Does those gauge pins ever wear out?

[@twoody2148]

maybe someone already asked , why would a desired off set of 1 thou (from 500 to 501)require like 6 thou offset ?

[@viharpatel8195]

T Woody : so, while using wear option I should put 0 in my (Haas) tool diameter offset?

[@lwilton]

So after all those burnishing cuts to walk in the hole diameter, what diameter hole do you get when you run the program from the start on a new hole?

[@steveh8724]

That is an excellent question! Why don't you try it and report back. Or have you in the last 12 months or so?

[@85CEKR]

The reason you get an alarm when your j value is smaller than the tool is because when using cutter comp you need a lead in distance long enough to allow the cutters path to compensate for the tools radius. I prefer to use wear because you can literally have a 0.01 thou lead in and it will still work (as long as the value in your tool offset is smaller). It allows you to use a much larger tool. The only problem is that you often have to use a negative value in your offsets. I'm not sure if path pilot will allow this. I would guess your Haas will though

[@occamssawzall3486]

Craig Krueger That’s what inverse wear offset is for. For machines that accept positive values only.

[@85CEKR]

I was wondering about that, how does that work?

[@occamssawzall3486]

Craig Krueger It works inversely to regular wear 😆 So instead of subtracting wear to make a hole bigger, you add wear to make it bigger. So if you’re at .002 wear and want the hole .001 bigger. You’d set the wear to .0025.

[@danmenes3143]

How does the controller know which side the cutter is cutting on? Do you have to do anything differently for conventional milling versus climb milling?

[@sp1nrx]

That is what a g41 or g42 is for. Those codes "tell" the controller what side of the path the cutter is on.

[@PaulSteMarie]

I've found that trying to use full tool diameter cutter comp is generally a bad idea. PathPilot may be catching some errors, but I've had Mach3 go off and do something crazy at times. The general problem is that gcode for boundaries just doesn't give enough information to be able to reliably calculate the offsets. It's not an issue if the offset is just 0.001-0.002" of negative compensation for cutter wear, but telling the control to apply say .125* of positive compensation and expect it to keep corners square, etc, is not a reasonable expectation.

[@danm3071]

It seems compensation type is limited to only 2d strategies is there any logic for this? I would think it should apply to 3d finishing strategies as well?

[@crazyg74]

Because you're delegating the calculation of tool offset to the CNC controller and it can only calculate left or right cutter comp in a single plane.

[@matthewcolvin4815]

Does path pilot have a way to use "wear" offsets or is "in control" cutter comp the only way path pilot adjust for variation in tool diameter.

[@No_Go_Moto]

Matthew I have the same question.

[@jmh1425]

Matthew Colvin I have used "wear" offset on my 440 from Fusion 360.

[@matthewcolvin4815]

Does anyone have a preference if cutter comp or wear offsets is better.

[@gredangeo]

Wear offsets. From my other comment: - I prefer to use "Wear" offsets, not "In Control" That way all your code is based from the center of the tool as normal. The key reason for this method is because in the Controller, all your offsets still say "0". You don't have to keep track of the tool diameter. (Accident waiting to happen). In your example John, you were going from .1875" to .1873". If you were using "Wear", you would put in -.0002". It's better to think about the toolpath as: 'Say, I want to push the wall further away from where it is. How far do I want to go? 'Negative Two Tenths'. *A negative value will remove material* Is a great way to remember it.

[@LizakDominik1988]

gredangeo True that, and pathpilot won't give you error message.

[@andrewgarrard4327]

Does the cutter comp work for the boring operation too or do you have to program a 2d contour to make it work?

[@oneflyvw]

CC works with boring operation. I prefer "wear" because the diameter entered into the controller is a small value (usually less than 5 thou), allowing the machine to engage cutter comp with a very small linking move which is very handy for boring.

[@longrangehunter6393]

I would be curious what that .501” bore really measures because of the intrinsic slop needed in order to fit the gage pin. Maybe measure it with your mitutoyo stand thing and update us on instagram what that says vs the actual diameter of the gage pin (mic’d)

[@Eggsr2bcrushed]

The hole is probably the slightest bit elliptical too because the CNC machine is not perfect. Overall I would bet within 2 tenths in diameter assuming the gage is a tight fit and exact size.

[@chiefmachining7972]

Well the holes is like .5015 ish because that was + size gage pin

[@mechfeeney]

raises hand

[@timmallard5360]

Any tips on how to get Fusion to post an "S" command at every operation. I find my self always editing the code at the controller and adding S3500 etc when I have to restart a program in the middle

[@sharmstr]

Hey Tim, I went to fix this for you in the post processor, but for some reason, no matter what I do, all my ops have a RPM callout. I could have sworn that this wasnt the case if the spindle speed didnt change between ops. So, now I'm thinking that maybe this was changed recently. What version of the post processor are you using?

[@timmallard5360]

I'm using the generic Tormach post from fusion. Maybe i need to get the updated one

[@sharmstr]

But what version? Open the post processor file. It will have a date near the top.

[@sharmstr]

FYI - The latest one is 12/13/17

[@MrJeffreyCHT]

The Rad in my tool data is easy enough to change without reposting a new program for a simple correction. Some of us, for cost savings, use regrinds and the diameter may vary more than .025 or more. So adjusting on the fly without waiting for a programmer to repost is much faster. In the old days of hand written programs they only program paths with radius called out, if I ran out of 3/4 endmills I could just change my tool radius in my tool data to a 5/8 and keep right on trucking. My point is some places are tying the hands of their cnc machinist and only trusting the programmer to make decisions, big problem when your pragrammer has 2 years experience and your cnc machinist has 15 years in his trade. And don't get me started on the programmer saying it should take 10 minutes to run a part...then on the machine it takes 15 minutes (but Y U take soo long).

[@kevingallineauii9353]

I wonder what the difference is in the g-code between "in comp" an "in controller"? Does one say move "the tool this way" and the other say "mill a round hole"? I am a complete novice at this and understanding the nuts and bolts helps me wrap my head around it. Having a background in computers has trained my brain to think in very abstract ways. Seeing the differences in the g-code would really help me get a firm grasp of the two ways to do this. It is literally easier for me to stumble through code many times. Great video though! I worked as a temp in machine shop that did a lot of large scale mass production. I sat by a machine for three whole days that did nothing but mill security lug nuts 24 hours a day. The CNC machine was about 30 years old and had a punch tape for a program (and this was over 10 years ago on top of that. The machine was old!). There was one variable, v20 I believe, that you would increase if i would remember correctly and that adjusted the tool path to account for tool wear. It was not the tool diameter, just a small number that would widen the "wobble" of the track the endmill would cut into the head of the nut. Having less than a month in any type of factory work and having never seen a CNC machine it was all facinating to me. Alas, after that job I spent the next 7 1/2 years doing little more than putting plastic parts on a box (cutting runners, counting them, etc). Good times.

[@natedawg003]

Both versions will always only say either go straight or go in an arc, that is the basis of g code. "In computer" programs the center of the cutter, which means the software adds the radius of the cutter to the dimensions it machines. "In control" programs the side of the cutter, the radius is added in the controller(by you) so the CAM software programs actual dimensions of your part. G code is just very basic computer code. I agree seeing and playing with the code helps a lot

[@kevingallineauii9353]

natedawg003 ok, does that mean that variable that john was changing around at CNC control would be set to "0" if the CAM operation was generated as "in comp" as it is already calculated by the CAM toolpath generated in Fusion 360? What I mean is there any parameter or que in the g-code that tells the controller "do not adjust for the tool size, we already took care of it". I know a lot of machine-specific variables and parameters can be passed via the post pocessor to the controller automatically (machine specific g-code numbers). Or, are most/all CNC machines "dumb" and you have to be careful not to double add(/subtract) an offset like a tool radius. It would seem the easiest way for John to do what he did in this example would be to always use "in comp" and then tweak the toolpath by inputing in the difference of the adjustment into that variable, ie -.0002 then -.0004, etc.

[@natedawg003]

If he's not using cutter compensation (g41 or g42) then it doesn't matter what value he has in the radius offset because it won't be taken into account. You have to include g41 or g42 to use cutter compensation. I would say CNC machines are "dumb" they only do what you tell them to do. The whole point of this video is to show another way to adjust your part. You can do it all in CAM, change the path and re-post, but that is tedious going back and forth. This way he is changing 1 value and rerunning, very fast and simple.

[@kevingallineauii9353]

natedawg003 ok, so there is a flag telling the controller to use an offset or not. I guess for more info I would have to read Pathpilot's documentation. I was somewhat familiar with LunixCNC (EMC CNC) but it has been a while. I am pretty sure I understand what he was doing at the controller now. Thanks for the replies.

[@VKRenato]

It is radius compensation.

[@occamssawzall3486]

VKRenato Diameter compensation. It’s a D value. And it literally says “Diameter” in the offset page.

[@NordicProspecting]

just change the diameter of the tool to make the hole smaller/bigger. smaller tool = bigger hole.

[@CodingCommunity]

Pop sound not recorded?

[@ikbendusan]

it just didn't make a pop, there's shit on his gage pin

[@M.L93]

I make something similar in haas vf2 with autodesk powermll and fuck the piece LOL

[@xenonram]

I like to think about what's going through your mind when editing. (Unless the young lady, who works for you, does it.)... Hmmm, what can I do to spice this up? I'll add "Pants on fire?"

[@oleksiylevenets8957]

ідеально, як по пісе лодошкою

[@Heizenberg.]

Am I the first to comment?

[@Nikolasz1173]

yes

[@Swarfman64]

lol, and you wasted it

[@Heizenberg.]

Swarfman64 I can edit anytime. 😎😎