Wear Comp effect Work Around?

[DanR]

In a different topic post an issue came up regarding tool comp.

 

Post comments included:

 

quote:

---

Edit/Delete Post Are you using wear comp?????

That way you use zero's in the geometry page of your control. One less thing to have to remember to change.

There are other advantages as well. Also...standard tooling in your machine will reduce the occurance of length offset errors.

They will already be set.

---

To this I replied:

quote:

---

I have been told I have to use 'control comp' since I have Renishaw Probes. Is this correct?

---

The response was:

quote:

---

No, the probe doesn't have anything to do with cutter compensation.

---

Today I tried to cut using wear comp. What apparently happens is that MasterCam X2 pulls a number from the Diameter Register on the offset page and offsets the cutter by that amount.

 

Without the tool probe, this register is apparently normally zero. With probes, this number is the actual diameter of the tool, (I would have thought that wear comp would have used the number in the tool wear column but oh well).

 

My part ended up WAY too big.

 

I checked the In House Solutions (Davis) book and the information there was consistent with what I observed. SO, I have to surmise that the probes DO in fact have a lot to do with the attempt to use wear comp (at least on a Haas). I called the local instructor who told me without hesitation that you can't use wear comp with a probe system on a Haas Super Mini; you have to use control comp. I reworked the file using control comp and reposted, and it cut perfectly.

 

 

Now the question! Losing the ability to kick a little wear into the tool to clean up the part by running it again is a pretty serious loss. I hate the thought of having to go back and offset geometry by .0005, reverify, repost, regraph and all to make another clean up pass.

 

Is there a work around that enables tool probe users to get the same effect as if they were able to use wear comp?

[YoDoug®]

I use wear comp in my Haas with a renishaw TS27R probe. when you call up the macro you have to preload the cutter diameter. I can't remeber which one it is but it is either the S or I value in your macro call. should look like this for .25 dia cutter.

 

G65 P9853 B3. T1 D1 S.25 I.25 Q3.

 

The o9853 macro needs to be modified to load the value from S, or I into the offset table, then after the tool is touched the macro subtracts the measured diameter from the preloaded dia. resulting in a wear comp. this is the beginning of our o9853

code:

---

(PRELOAD TOOL DIA.)

#[#20+2400]=#19

---

I also have my post in MCX set up to use misc interger 5 to add tool setting to my posted program. I enter a 1 (in misc5) to touch length, a 3 to touch length and dia, or a 4 to touch lentgh without offsetting tool for large diameters ( for drills bigger than 10mm). this is what the posted code looks like. (/block delete so you can skip tool setting after first piece)

 

code:

---

(  1/4 FLAT ENDMILL | TOOL - 1 | DIA. OFF. - 1 | LEN. - 1 | Dia. - .25 | | )

T1 M6

/ g103 p1

/ G65 P9853 B3. T1 D1 S.25 I.25 Q3.

G0 G90 G54 X-.9829 Y-1.4234 A0. S7500 M3

G43 H1 Z2.

---

Send me an email if you like and I can help you with the correct changes to your macros.

[Guest]

In all of my dealing using probes I have NEVER used any type of comp on them what so ever.

 

All G65 macro calls from a custom drill dycle but never a comp move to be found.

[YoDoug®]

The probe I was referring to was the tool setting probe, not the spindle probe.

 

With the spidle probe there is no comp involved.

[YoDoug®]

:hijack:

 

JP, have you ever set up a lathe post to use custom drill cycles for a turret probe. We have a Renishaw probe in one of our lathes that I use renishaw inspection plus lathe macros. Currently I have four inspection cycles that I cut and paste into a manual entry tool paths and edit the variables in the G65 call. Easy to make mistakes this way.

 

Custom drill cycles seems like a better idea to me.

[Guest]

No I haven't.

 

I don't "think" there would be a problem however let me dig a bit.

[heeler]

quote:

---

Now the question! Losing the ability to kick a little wear into the tool to clean up the part by running it again is a pretty serious loss. I hate the thought of having to go back and offset geometry by .0005, reverify, repost, regraph and all to make another clean up pass.

 

Is there a work around that enables tool probe users to get the same effect as if they were able to use wear comp?

---

This is the whole purpose for have cutter comp. Reguardless of using full or wear. If you need to comp the tool from the measured/nominal/zero dia. you just adjust the amount of the comp. You will have to either just measure the tool ate the beginning of the job, or find a way to have the control adjust the measured value when it measures it the second time.

 

HTH

 

Glenn.

 

P.S. What I mean is if you use full comp. and the machine measures the tool at .4998, and you need to take .005 more off of the profile of a part, you will change the comp value to .4973, unless your control uses radius, then you would change it to .4948

[ARP]

DanR,

Make sure your HAAS is using Diameter in the offsets.

Program in Mastercam with nominal tool sizes like .125, .25, .1875 whatever size using WEAR.

When you touch off the tool, don't set the diameter, just touch off for length comp.

In the Wear column of your offsets punch in how much wear you need to achieve a desired size after you have measured the part and determined how much you need off.

If you use Wear when you program in Mastercam and you have a diameter value in the diameter column of your HAAS offsets you will have huge comp. Make sure your program has a D in it to pickup your wear comp value and probably some small straight line perpendicular move to pickup the D before cutting and you should be good.

After making first cut with no wear (nominal cutter size taken care of in Mastercam) and measuring your part you know what number to punch in your WEAR column in offsets.

[Guest]

Doug,

 

I am going through a post, the generic 2-4 axis post and if your machine has mill capabilites, then you can drill and if you can you have access to the custom drill cycles, so yeah it would be something that could be done.

[YoDoug®]

Yeah JP, its a single spindle XZC+live tooling. I thought it would be possible. I remember a post a while back that discussed setting up custom cycles for a mill post. I'll reference that if needed.

 

Thanks

[DanR]

After some further research, Heeler had it right on, and ARP was right too. Getting the tool diameter as a comp is a real surprise. I ended up using "Control" but got the same results with compensation type "off".

 

I got the same effect as bumping up the tool wear by telling the machine the tool was a little smaller than it was, just like Heeler said. I even caught the fact that if I wanted to take .001 that I had to take half off each side on the closed contour cut.

 

DS, I found that Haas had sent me some code for a VQCPS and put a WIPS on the machine. The Visual Quick Code didn't work, and there were problems with the IPS. A new install made things work a lot more reasonably. Now the world is good!

 

Thanks, Dan

 

Thanks all!