[kentdesautel13]

In my Cam Software ( Fusion 360 ) I typically use a nominal tool diameter ( example for my 1/2" would be .50 " ) verses the exact measurement of the tool at that point in time.

What I would like to do is make my adjustments on my Haas classic controller.

So my understanding is that in Fusion I change the compensation type to " In Controller "

My question is my setting on the Haas.

For this example In Fusion my tool diameter is set at .500 "

My actual tool diameter on the machine after probing is .5015"

I believe my machine compensation is setup for diameter verses radius

So would I set my wear compensation for that tool as a positive .0015?

Second question, since my tool probing already put the .5015 value in for the tool diameter do I just leave that in there? ( In other words is the machine using that value for calculating, or is it just to reference?

Thanks for any advice on this....

Kent

[Donkey Hotey]

My actual tool diameter on the machine after probing is .5015"

I believe my machine compensation is setup for diameter verses radius

So would I set my wear compensation for that tool as a positive .0015?

No, you don't enter any adjustments or change anything. That's the whole point of having control compensation and the tool setter. Wear is zero unless you still aren't getting the size you need and want to fudge it larger or smaller. If the tool is 0.5015, leave it. 0.500 in Fusion is fine.

I haven't programmed in Fusion but, hopefully it forces you, or you know, that you have to ramp onto and off of the part profile. That usually looks like a right angle approach and maybe an arc onto the part profile. The control has no way of knowing whether it needs to turn right or left when it gets to the part and it figures that out during the entry move.

Related: 0.5015" sounds suspicious. Have you calibrated your probing system recently? Endmills almost always come in undersize. The shank is usually ground right to nominal (0.5000) and the flutes eat a little off that. I suspect the probing is not calibrated or you have a ton of run-out in the holder. If you have 0.002" of run-out, some flutes may be eating 0.004 and others taking nothing.

[Superman]

There is a few choices that apply to compensation methods

-Off .... CAM doesn't output comp codes, path is "locked" to what was set on-screen.
-in Control .... CAM outputs toolpath on top of selected geometry. You tell the control how much to offset
-Wear .... CAM outputs a path that is 1/2 your selected cutter diameter. Any +ive offset in the control moves the path away from your geometry. Any -ive value makes the cutter path closer
-Negative Wear .... never used, so can't say

Note.... the value placed into the control cannot be larger than any inside radius on your toolpath, as it would in effect skipping that bit.... you would get an error, and processing would stop.

IMO .... I would consider WEAR, as you would not need to have a offset value other than zero in the control to have correct working NC code. Result.... less scrap....
.... Unless you put in a larger tool than what was programmed.

[Donkey Hotey]

IMO .... I would consider WEAR, as you would not need to have a offset value other than zero in the control to have correct working NC code. Result.... less scrap....
.... Unless you put in a larger tool than what was programmed.

He's using Renishaw probing on a Haas. The diameter values are loaded straight into the Geometry column. There are no problems unless he starts moving values around and changing things. Preset the tool, use Control Comp, run the part. Wear requires knowing both what was programmed in the CAM and knowing what the presetter thinks it is. All kinds of chances for mistakes.

[kentdesautel13]

Thank You very much for the great Info... It has been some time since I calibrated the tool setter, so that is on tomorrows To-Do list.

I followed your suggestion and removed the figures in the wear column re-checked the diameter with the tool setter and it made a huge improvement.

Yes, Fusion has the ramping, along with all the options for the entry.

Thanks again for the info.

Kent

[Donkey Hotey]

When you do the calibration of the presetter: make sure you've indicated it flat to the spindle with a tenths indicator if you can. Next, make sure you use a micrometer good to tenths to measure your reference shank diameter.

I usually use the butt of an old endmill, spun around backwards in a holder. They usually measure a few tenths under 0.5000". The accuracy and care you do during those steps will drive all your sizes from there on.

For reference, brand new Niagara carbides in the machine right now: 1/4 comes in at 0.2477 and the 1/2 at 0.4982. That's why I questioned yours coming in oversized. It has to be out of calibration or really off center.

[kentdesautel13]

Hi Greg,

Just a couple of quick follow up questions.

After re-calibrating everything on the machine, and doing some testing of that haas brand ( maybe the issue? ) 1/2 inch end mill it looks like it's cutting diameter is .5007

How I arrived at this is by first making sure my probe is reading accurate ( I did this my checking it against a 1.0000" gage, and the probe was dead on.... so that was good news )
I wanted to make sure my probe was reading accurate so I could check my machined work piece to check accuracy.

So next I machined an outside finish pass on an aluminum block with a target x axis measurement of 7.99"

on my 1/2 end mill I started with larger diameters and kept decreasing till I got near my 7.99 target

.5009 = 7.9917
.5008 = 7.991
.5007 = 7.99079

My haas will only let me key in a 4 digit diameter, is it possible to change a setting to allow 5 digits? This would allow me to get it dead on?

Or maybe I should change my setting from Dia to Radius on the machine wear compensation to allow me to dial it in closer?

Maybe I'm being too anal on this.... but I'm still getting a little offset edge on the side of the work piece when I flip the piece over and do the second pass.

Thanks,

Kent

[Donkey Hotey]

Kent,

To be clear: I use the shank of an endmill, measure it to the tenth or maybe half a tenth if I think that's where it really is. I do that with a micrometer, use that for the keyed value during the calibration and I move on. If you're changing diameters in the offset screen trying to make adjustments, that's where you should be using the wear column to add/subtract to adjust the cut. To keep things straight, the Geometry value should be what the presetter recorded.

As for side-to-side mismatch, you'll probably never get that perfect but, are you probing a reference surface machined during the first op or just putting it up to a work stop? I've had absolutely crazy-accurate results from cutting a reference datum and picking that up with the probe on the flip. So close that the mill marks made a basket weave pattern on the ends of the part. But that's with freshly cut soft jaws or absolutely dead-zero runout from your jaws.