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'.

[@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.

[@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.

[@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.

[@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.

[@LizakDominik1988]

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

[@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.

[@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

[@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!

[@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.

[@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

[@twoody2148]

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

[@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.

[@OakwoodMachineWorks]

YES! THANK YOU JOHN!

[@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

[@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

[@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..