Help Understanding "Walking It In"

TheWolfOfWalmart · Apr 1, 2019

Hey all. First post since I got my 2016 Mini Mill and have been burning the candle on both ends studying this arcane art.

One thing I haven't been able to understand completely yet is what everyone keeps referring to as walking in a dimension with cutter compensation, e.g. tight tolerance bore diameter, slot width, etc...

What exactly is the generally accepted work flow for this? Roughing op > contour > measure > edit cutter comp value > another contour? Just one contour op but stop > edit > re-run? I'm sure there is a lot of ways to go about this but I'm positive there is a better way than I've been doing it.

What do you guys do?

Thanks!

Hazzert · Apr 1, 2019

Normal procedure around here for a tight feature would be to rough it out, plus comp the finishing tool, measure the feature and adjust compensation for the difference between actual and ideal and then rerun the feature.

Keep in mind that running the feature again will cut differently than finishing the feature with the roughing stock allowance on it.

TheWolfOfWalmart · Apr 1, 2019

Thanks for the reply. To clarify on your second paragraph, are you just saying to mind my "stock to leave" value on my adaptive/roughing op after I've changed my cutter comp value?

Hazzert · Apr 1, 2019

Say you are cutting a Ø1 hole. I would rough the hole to Ø.98" (.01" per side allowance) and add .005" D comp to my finisher on the control then take a cut and measure the hole at .996" (for example) I would then remove .004" of D comp and rerun the tool. However that will cut differently than .01" per side finishing allowance and .001" comp on the tool due to deflection or other factors.

gkoenig · Apr 1, 2019

TheWolfOfWalmart said:
What exactly is the generally accepted work flow for this? Roughing op > contour > measure > edit cutter comp value > another contour? Just one contour op but stop > edit > re-run? I'm sure there is a lot of ways to go about this but I'm positive there is a better way than I've been doing it.

That is pretty much the procedure.

In production, one would do this once to dial in a tool on a particular feature, then let it run while checking every X number of parts to keep babysitting it. You chase both thermal shifts in the machine + tool wear, so an aluminum part doesn't need to be checked all that often, 4140HT way more. You eventually build up some internal knowledge of what exactly is going to work.

Best practice is to program cutter comp so that the code is programmed to the nominal tool diameter, and you are just inputting wear values (most shops are not coding to the tool centerline and using cutter comp to walk the tool out the full radius).

One trick is to put a few lines of code at the end of the contour with block skip on them; with block skip turned off, the machine stops at the end of the contour and brings the part to the door for you to measure. You make adjustments, hit cycle start, and the next line of code is a GOTO that jumps back to the beginning of the contour and runs it again. On the next measuring cycle if the part is good, you turn off block skip and hit cycle start and the machine carries onto the next set of operations. Gives you an easy way to do this on production code, especially if you need to change end mills often and dial them in again quickly.

TheWolfOfWalmart · Apr 4, 2019

Ok I get what you are saying- Thanks for the clarification

TheWolfOfWalmart · Apr 4, 2019

gkoenig said:
That is pretty much the procedure.

In production, one would do this once to dial in a tool on a particular feature, then let it run while checking every X number of parts to keep babysitting it. You chase both thermal shifts in the machine + tool wear, so an aluminum part doesn't need to be checked all that often, 4140HT way more. You eventually build up some internal knowledge of what exactly is going to work.

Best practice is to program cutter comp so that the code is programmed to the nominal tool diameter, and you are just inputting wear values (most shops are not coding to the tool centerline and using cutter comp to walk the tool out the full radius).

One trick is to put a few lines of code at the end of the contour with block skip on them; with block skip turned off, the machine stops at the end of the contour and brings the part to the door for you to measure. You make adjustments, hit cycle start, and the next line of code is a GOTO that jumps back to the beginning of the contour and runs it again. On the next measuring cycle if the part is good, you turn off block skip and hit cycle start and the machine carries onto the next set of operations. Gives you an easy way to do this on production code, especially if you need to change end mills often and dial them in again quickly.

Thank you! This is definitely the smarter-way I was looking for. Luckily I have the perfect project coming up to try this on. Can't wait

TheWolfOfWalmart · Apr 4, 2019

gkoenig said:
Best practice is to program cutter comp so that the code is programmed to the nominal tool diameter, and you are just inputting wear values (most shops are not coding to the tool centerline and using cutter comp to walk the tool out the full radius).

So would this be achieved modifying the diameter probing cycle on my WIPS tool probe?

Delw · Apr 4, 2019

on a hass you dont need to just type in

G01 Z-0.5 F50.0 Assumeing there is a predrilled hole bigger than your endmill
G13 I0.2 k0.490 Q0.010 D1 F15.0 I= start hole size K=finish Hole size Q= amount of step over (the G13 is a spiral) D= tool dia offset
G00Z0.5

I's and K's are rads NOT DIA

if you just want to bore it then:

G01 Z-0.5 F50.0 Assumeing there is a predrilled hole bigger than your endmill
G13 I0.5 D1 F10.0
G00 Z0.5

Delw · Apr 4, 2019

TheWolfOfWalmart said:
So would this be achieved modifying the diameter probing cycle on my WIPS tool probe?

no leave that alone till you know what your doing. one crash $1200 plus downtime.

you can write a macro so that your probe will measure the dia an adds what is needed to the program. its complicated, I think it was Ynda(sp) that did it on another board a bunch of years ago

Delw · Apr 4, 2019

Oh my reply was to he was talking about a Haas mini mill, if not disreguard

TheWolfOfWalmart · Apr 5, 2019

Delw said:
no leave that alone till you know what your doing. one crash $1200 plus downtime.

you can write a macro so that your probe will measure the dia an adds what is needed to the program. its complicated, I think it was Ynda(sp) that did it on another board a bunch of years ago

Yeah I remember reading somewhere that someone changed all their probing macros so that the diameter in the offset tables were zero'd out(with the nominal diameter taken into account) so that all you needed to do was add wear values. But perhaps I misunderstood. Either way though, you're right- I don't think I'm quite there yet lol.

Delw said:
G01 Z-0.5 F50.0 Assumeing there is a predrilled hole bigger than your endmill
G13 I0.2 k0.490 Q0.010 D1 F15.0 I= start hole size K=finish Hole size Q= amount of step over (the G13 is a spiral) D= tool dia offset
G00Z0.5

Ok it sounds like there is more to G13 than I thought. I'm going to go read up on that again. Thanks for the tip!

Search

Largest Manufacturing Technology Community on the Web

Search

Help Understanding "Walking It In"

TheWolfOfWalmart

Plastic

Hazzert

Stainless

TheWolfOfWalmart

Plastic

Hazzert

Stainless

gkoenig

Titanium

TheWolfOfWalmart

Plastic

TheWolfOfWalmart

Plastic

TheWolfOfWalmart

Plastic

Delw

Stainless

Delw

Stainless

Delw

Stainless

TheWolfOfWalmart

Plastic

Similar threads