"Qualifying" a cutter versus using cutter compensation.

implmex · Jan 21, 2017

Hi All:
What is your preference when you have to make a very accurate 2D feature...say a simple rectangular pocket, but it must be as accurate as you can mill it?
You're only going to do this one feature super accurately and you'll only make one or a very few parts.

My business partner Keith uses a procedure where he will make test cuts to find out how big his cutter is actually cutting, then he edits the cutter size in the CAM program (we are using HSM Works) and then he posts his code and cuts, assuming his part will be on size.
One finish cut, one time and if it's wrong...it's a tosser.
But if it's right, it's only one cut.

I, on the other hand, will program with wear compensation in the control, leaving a couple of thou stock and then increase the comp in two increments, the first to establish how much stock is left, the second to bring the pocket to final size, and if I need truly super accuracy, some spring passes; as many as I need to bring the part to size, gauging as I go with Jo blocks or whatever is appropriate.
One finishing program, run as many times as necessary to sneak up on my dimension and maintain control.

When you have features like this that must be right on the money, do you prefer Keith's way or mine?
Why do you choose the method you prefer?

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

Atomkinder · Jan 21, 2017

Wear comp, second option.

Why chance scrapping it when it can be comped ten thou big and snuck up on? For critical features I frequently program a spring pass after two same-size finish passes. Also using HSMWorks, and in 2D Contour this is very very simple to do.

Finegrain · Jan 21, 2017

The cutter only cuts a specific size for:

1. Specific material (even different batches can cut different)
2. Coolant condition
3. Tool life
4. machine warms up or cools down
5. probably several other factors

No sense in trying to dial in the CAM each time one of these changes. Tell the CAM to leave .002" on the walls/floors then dial it in at the control with wear comp. IMO anyway.

Regards.

Mike

BALNH · Jan 21, 2017

Plop some positive comp in wear. I program so what I know what finish allowances are, but enough comp allow to cover finish allowance. Then run, measure, run again. I will mill super tight pin holes/bores like this. Also works for bosses or external features. I know someone will say bores arent round but the customers haven't complained and they come back for more.

allloutmx · Jan 21, 2017

in the 5th, may qualify the tool that cuts the perimiter with a z and y cut before I adjust the wear. once I establish my Z is where it needs to be, I will then rotate the part so that i am approaching the feature in Y direction and adjust tool comp until you begin to tickle your Z cut. This tool is now qualified and So long as you already know you are machining about center you can trust your other part features to be measured off of the features you cut using the qualified tool.

Also-have come to learn to check the values that cam posts out to ensure they match print numbers. Rounding errors in CAD/CAM will play havoc when you get into the tighter tolerances

wrustle · Jan 21, 2017

We run two separate tools.

T16 our .500" Carbide End Mill always profiles or pockets to allow .005" on sides, or in bores (if critical).

T17 our .500" Finish Carbide End Mill always takes the finish pass on the profile, pocket or bore, and we seldom if ever have to dial it in, as it always removes the same amount of material, but even then.........we use cutter comp to control size if or when it is necessary, but typically it's right to size, every time!

Once we start having any sort of taper issues T17 then gets moved to T16, and a new T17 is put in the machine, dialed in on the next fussy job, and it will be good to go for a long, long time!

We've done this for years with great results!

Later,
Russ

706jim · Jan 21, 2017

wrustle said:
We run two separate tools.

T16 our .500" Carbide End Mill always profiles or pockets to allow .005" on sides, or in bores (if critical).

T17 our .500" Finish Carbide End Mill always takes the finish pass on the profile, pocket or bore, and we seldom if ever have to dial it in, as it always removes the same amount of material, but even then.........we use cutter comp to control size if or when it is necessary, but typically it's right to size, every time!

Once we start having any sort of taper issues T17 then gets moved to T16, and a new T17 is put in the machine, dialed in on the next fussy job, and it will be good to go for a long, long time!

We've done this for years with great results!

Later,
Russ

This is probably the best way suggested so far. From my experience, if you're just doing one part, I would use G41 (or G42 sometimes for mild steel strangely enough) and run a finish pass or two to get to size. But doing this method for multiple parts isn't necessarily going to give you consistent sizing as the tool wears or has to cut a greater amount. All cutters bend a certain amount under load which can lead to size inconsistencies.

CarbideBob · Jan 21, 2017

I can only machine a pocket within a tenth or three. Not sure what you consider tight.
If one off I'll program with the spring passes leaving leaving .002/.003 in the CAM side.
Then measure, change the amount of stock to leave in the CAM even if minus, send the finish passes only to the control and hope I can reload the part within a tenth.
I only change tool D or wear offsets to comp on longer runs but we are setup for operators to repost the CAM output for a part in less than a minute which is not the norm. Mcam is open on every part being run on the other computer at the workcell and waiting for tweaks be it feed rates or size.
I'm not so trusting of test cuts unless they are the same geometry and slide positions as the real thing.
Certainly gives you a good idea of where you are and a step better than a tool presetter but no machine is right on in axis travel.

Both ways work if you have room, both take some time. One has more risk on a one off.
Easy to take more steel out, hard to add it back on.
Any possible error or oops in the process or procedure should be intentionally directed at the plus material side on small lots.
Not great Ppk numbers offset this way but you save parts in the small run world.
Bob

Dave K · Jan 21, 2017

Wear comp was made exactly for this reason. You can sneak up on your size, and you can also adjust as the cutter wears from one part to the next, if there's multiple parts.

Zahnrad Kopf · Jan 21, 2017

This is a subject that is actually a topic of consideration right this minute, here. For almost a decade, I have done it the way that your partner is doing it. Now you know this already, but for the sake of discussion I will point out that my life is very much made of parts that occur in quantities of only one or two. Some times there might be three or five, but the vast majority are onesy/twosy. Like I wrote, I've always done it your partner's way.

However, ... ... ... with the caveat that performance was tracked and sizes could reliably predicted in similar materials and shapes with similar cutting styles and chip loads. When something out of the normal was encountered, it was programmed ( as others have suggested ) to finish up a few thou oversize, and the result measured for accuracy. Then it was adjusted in CAM and run again to clean up.

Lately, however, since I installed the Probing and Tool Setting system I have been considering telling the CAM to let the machine control the offsetting and do it the way you propose. Especially since the Renishaw will do both length and diameter automagically and I have become fond of checking them during the program for not only breakage, but wear, as well. In light of that, I have to admit that I'm more and more every day liking the latter more than the former.

DMF_TomB · Jan 22, 2017

implmex said:
Hi All:
What is your preference when you have to make a very accurate 2D feature...say a simple rectangular pocket, but it must be as accurate as you can mill it?
You're only going to do this one feature super accurately and you'll only make one or a very few parts.

My business partner Keith uses a procedure where he will make test cuts to find out how big his cutter is actually cutting, then he edits the cutter size in the CAM program (we are using HSM Works) and then he posts his code and cuts, assuming his part will be on size.
One finish cut, one time and if it's wrong...it's a tosser.
But if it's right, it's only one cut.

I, on the other hand, will program with wear compensation in the control, leaving a couple of thou stock and then increase the comp in two increments, the first to establish how much stock is left, the second to bring the pocket to final size, and if I need truly super accuracy, some spring passes; as many as I need to bring the part to size, gauging as I go with Jo blocks or whatever is appropriate.
One finishing program, run as many times as necessary to sneak up on my dimension and maintain control.

When you have features like this that must be right on the money, do you prefer Keith's way or mine?
Why do you choose the method you prefer?

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

.
.
wear comp is much easier and faster as cutter wears and comp can be adjusted -.0001 in a few seconds

SND · Jan 22, 2017

I do it in CAD/CAM because I haven't practiced much with the wear comp thing. I also don't do much under .005 tolerance in the VMC anyway and I already know which endmills to input at .123" or .4985" to almost always get it within .001" anyway. With the way endmills are ground, cut deflection, run out, machine positioning accuracy, etc anything much below .001" with any real length/depth is pretty much a fantasy anyway. Like people who try to interpolate bearing bores in stainless with +.0003"-.0000 tolerances... not me.

DMF_TomB · Jan 22, 2017

SND said:
I do it in CAD/CAM because I haven't practiced much with the wear comp thing. I also don't do much under .005 tolerance in the VMC anyway and I already know which endmills to input at .123" or .4985" to almost always get it within .001" anyway. With the way endmills are ground, cut deflection, run out, machine positioning accuracy, etc anything much below .001" with any real length/depth is pretty much a fantasy anyway. Like people to try to interpolate bearing bores in stainless with +.0003"-.0000 tolerances... not me.

.
.
fairly standard cutting slots to use gage blocks and check if go in slot all the way. most of what i cut is less than .0005" tolerance. you can measure with different gage blocks if slot parrallel sided to .0002" basically like a go and no go gage. number one rule is to use a separate cutter for finish milling as roughing cutters are often badly worn in corners
.
circular milling often machine will not cut round to less than .0010" thus why boring bars are still used to get +/-.0001" tolerances. it is true some material are easier to machine to finer tolerances. cast iron often machines quite nice

SeymourDumore · Jan 22, 2017

Marcus, I am with you on using comp all the way.

In fact, I am anal about it to a point that even the roughing op is comped every single time without exceptions.
There is no way in hell would I ever re-post a code just to dial in a feature size.

Not only that, but when the same tool is used to finish different features which are tight and of incosistant leftovers ( say a boss that's roughed and vs a drilled hole to be finish interpolated)
I program separate diameter offsets ( D-word ) for each feature.

But that's just me ....

CarbideBob · Jan 22, 2017

SeymourDumore said:
I program separate diameter offsets ( D-word ) for each feature.
.

One wonders why people consider wear comps and D numbers as different things.
The control just adds them up to a number it uses to shift off the programmed path.
Wear comp handy but no different than a D change.

I just prefer to re-post to bring in a size as it is easier with my setup and takes under 30 seconds but my CAM and CNC controls speak at 100Mbps and the cnc "sees" a new program coming in so not normal.
On a standard Fanuc or other cnc I'd probably do it much differently so my view is skewed.
I hate lost seconds so it depends on your arrangement.
Fast is good, risk of scrap is not so good. One overcut per year erases many, many seconds of time saved.
Often people go for fast and sort of overlook the rare oh-chit and how much it really costs.
You think you won't repeat this mistake.... then next year you do it and you think never again.....
Bob

rlockwood · Jan 22, 2017

CarbideBob said:
One wonders why people consider wear comps and D numbers as different things.
The control just adds them up to a number it uses to shift off the programmed path.
Wear comp handy but no different than a D change.

wear comp and wear offset column are two distinctly different things. In traditional cutter compensation use, the toolpath is not offset from the geometry, and relies upon the diameter offset value to perform the offset. In wear compensation, the toolpath is offset via cam, but cutter compensation is still issued. Therefore, with a zero offset register, the toolpath is still valid, and you need only input correction into the offset table.

To the OP.. I do both, so not much help here.. But, primarily, I prefer to keep a clean CAM tool library, so you won't find tools with odd diameters there. Usually, I tweak via stock to leave instead, but there are just instances where I know i'll want to dial something in at the control and sneak up on it, and for those CC is easier.. And then there's critical 3D surfaces, and lying to CAM is easier there.. And so on.

Orange Vise · Jan 22, 2017

I'm with you, Marcus. Comp it. Why spend extra effort and material making test cuts?

On a critical feature, comp the cutter to +0.002" and run the program. Measure, comp, and rerun the finish pass + spring pass. Minimal effort required to turn on the optional stop and rewind a bit.

Chances are you'll have to comp the tool again anyway, possibly multiple times, as it wears and when it gets replaced.

Cutters behave differently in different toolpaths anyway. The required offset in a test cut could be different than the offset in the actual part, even with the same material with the same parameters. I would not trust test cut results in a different workpiece if I were trying to hold a few tenths.

NAST555 · Jan 23, 2017

implmex said:
Hi All:

I, on the other hand, will program with wear compensation in the control, leaving a couple of thou stock and then increase the comp in two increments, the first to establish how much stock is left, the second to bring the pocket to final size, and if I need truly super accuracy, some spring passes; as many as I need to bring the part to size, gauging as I go with Jo blocks or whatever is appropriate.
One finishing program, run as many times as necessary to sneak up on my dimension and maintain control.

Pretty much how you do it. I let them CAM work out the toolpath with my cutter size (so no tool dia at the machine) and start off with a positive number in my wear offsets at the machine roughly half of what I left from roughing. Take the first finishing cut and measure and use the wear at the machine to dial it in for the last cut and run the finishing again. Obviously pretty often my wear offset lands up to be a small negative value.

For one,two or three off's before I cut the next one I will return to a positive value before I cut the next part so I can dial it in again just to make sure and since I am leaving in theory double the amount after roughing if I try to take it in one cut there is a good chance that the sizes will be off.

I find it easier than having to go back to the CAM and editing it there for each cut.

WILLEO6709 · Jan 23, 2017

The only time I have qualified a cutter is those times where you have to destroy a part to get to the feature to inspect it easily. I have run into t slots etc that are not open on each end and have a function check but for first article etc. a part has to be sectioned. You section it, check all your features, " qualify your code", then use comp for width etc.

With theadvent of scanning cmm( which I don't have) its getting rarer.

apoc_101 · Jan 23, 2017

I use both techniques and the reason to use Comp in control is simple: do you want to avoid scrap on a high tolerance part, or not?

Otherwise I let my CAD/HSM files stay in charge. the tooling doesn't change, the material for production parts doesn't change, this way, if the program needs to be re-posted, the size won't change either (which maintains how things fit together later in production). It also just so happens my speeds and feeds are actually right in the posted programs (unlike 99% of programmers I've ever met.)

"Qualifying" a cutter versus using cutter compensation.

Diamond

Titanium

Diamond

Cast Iron

Titanium

Titanium

Titanium

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Stainless

Titanium

Stainless

Diamond

Hot Rolled

Similar threads