Mini-mill offset questions.

[kutter]

Hi All,

I have a Mini-mill that i purchased in 2001, and have used it everyday since.
Its a great machine and not one problem since it was installed.

My question is regarding the offsets page. ... i think.
I make custom knives for a living, most of which have inlays. After cutting
the pocket in the frame of the knife, I cut an inlay to fit. What i would like to do is change the size of the inlay by .001 or .002" without having to reprogram the part. I've experimented with the available inputs regarding tool wear and diameter inputs on the offset page. To no avail. I'm sure I'm just missing something. Any help would be appreciated.

Regards,
Jeff

www.customknives.net

[dcoupar]

Are you programming a G41 (left) or G42 (right) to activate the cutter comp? The values in the Geometry and Wear offsets don't do anything unless cutter comp is activated. Usually, roughing is done with comp off, and then comp is turned on with a feed move to the start of the finish profile.

[Donkey Hotey]

Did you program the parts with cutter compensation or without? Changing the diameter and wear offsets will have no effect if you didn't program using cutter comp.

Edit: damn, too slow on the draw.

[kutter]

Hi Guys, Thanks.

The roughing is done with comp off and the finish pass has it on. At least that is what camworks says. I'm not sure that clears anything up. I don't know a lot about the actual code. Ie. g41/g42...

Thanks,
Jeff

[Pondo]

If you are climb milling (should be), the the CAM should use a G41 to turn on the comp. The D callout in the line should correspond to the tool you are using. Sometimes if the tool data in the CAM program is not correct it will not put the correct D in the program (common in Mastercam). The controller usually is set to alarm out if the H and T #'s don't match, but it will let the D callout be whatever.
The comp you want to change in the controller can be either the tool geometry or tool wear offset.
The amount of the adjustment depends on how your machine is set up, either to read as the tool diameter or the tool radius.
If you have a sample program and post it here, I'm sure someone will be able to point out any issues it may have.

PS-Your knives are absolutely beautiful! Do you do the handle engraving by hand or in the machine?

[dcoupar]

Why not post the section of code that shows the finish profile here so maybe we can help... Also what values are you putting in the geometry and wear offsets?

[kutter]

Thanks again, guys. My ignorance is showing through. Thanks for the kudos Pondo, yep all the engraving is done by hand, under a stereoscope.

Here is the Haas code for 2 inlays, direct from camworks. I see a D23, although i have know idea as to its meaning. I assume Diameter. I currently
haven't been useing anything in the Dia., wear, registers at least since my early trail and error testing.

So this is the code for 2 inlays, programed as bosses and listed under contour mill. Climb milling in effect. Just to be clear, I would like to shrink or grow the inlays without reprogramming, via the D? offset. Or maybe my .093 is really .091" and i want to compensate in the machine. I reckon that's a bit clearer. Could there be an issue in my post, or a switch on the machine?



Thanks again,
Jeff


%
O0001
N1 G00 G90 G49 G20 Z0
N2 T03 M06 (3/32 2 FLUTE HSS EM)
N3 S6000 M03
N4 G00 G54 X3.0238 Y.4681 S6000 M03
N5 G43 H03 Z.1 M09
N6 G01 Z-.125 F2.
N7 G41 D23 X3.0424 Y.4606
N8 X4.3085 Y.4197 F10.
N9 G02 Y.1284 R.1457
N10 G01 X1.7863 Y.0468
N11 G02 X1.7029 Y.0699 R.1449
N12 G03 X1.4887 Y.063 R.188
N13 G02 X1.407 Y.0345 R.1448
N14 G01 X.307 Y-.0011
N15 G02 X.1762 Y.0725 R.1449
N16 G01 X.1027 Y.2028
N17 G02 Y.3452 R.1448
N18 G01 X.1762 Y.4755
N19 G02 X.307 Y.5491 R.1449
N20 G01 X1.407 Y.5135
N21 G02 X1.4887 Y.485 R.1449
N22 G03 X1.7029 Y.4781 R.188
N23 G02 X1.7863 Y.5013 R.1449
N24 G01 X3.0524 Y.4603
N25 G40 X3.0714 Y.4666 F2.
N26 G00 Z.1
N27 X3.0216 Y1.0335
N28 G01 Z-.125 F2.
N29 G41 D23 X3.0402 Y1.0261
N30 X4.3062 Y.9851 F10.
N31 G02 Y.6938 R.1457
N32 G01 X1.7841 Y.6122
N33 G02 X1.7007 Y.6354 R.1448
N34 G03 X1.4864 Y.6285 R.188
N35 G02 X1.4047 Y.6 R.1449
N36 G01 X.3048 Y.5644
N37 G02 X.1739 Y.638 R.1449
N38 G01 X.1004 Y.7683
N39 G02 Y.9107 R.1448
N40 G01 X.1739 Y1.041
N41 G02 X.3048 Y1.1146 R.1448
N42 G01 X1.4047 Y1.079
N43 G02 X1.4864 Y1.0505 R.1449
N44 G03 X1.7007 Y1.0436 R.188
N45 G02 X1.7841 Y1.0667 R.1449
N46 G01 X3.0501 Y1.0258
N47 G40 X3.0692 Y1.032 F2.
N48 G00 Z.1
N49 G91 G28 Z0
N50 G28 X0 Y0
N51 M30
%

[Matt@RFR]

Let's try and clear this up for you:

Txx = The physical tool that you are using.

Hxx = The length offset for that tool. There is a geometry and wear column in the offsets page for this.

Dxx = The diameter offset for that tool. Again, geometry and wear columns in the offsets page.

In your code, you have T3, H3 and D23. For now, let's ignore the fact that this is possible, to make it simpler. Change the D23 to D3 so everything matches.

At this point, we need to know if you are using geometry or wear compensation in your CAM program. Your software might call these things by different names.

If you are using wear comp in CAM, then in the offset page, your geometry column should be zero, and any adjustments to the tool diameter will be in the wear column. If your part is .005" too big on the outside, then an entry of -.005" in the wear column will get you close.

If you're using geometry comp in CAM, then the geometry column in the offset page should have your nominal tool diameter entered, and any adjustments should be made in the wear column, same as above.

The code "G43 H3" forces the control to look in the geometry and/or wear column for tool 3, under the height offset. It then uses the numbers you have entered to compensate for the tool's actual length.

The code "G41 D3" forces the control to look in the geometry and/or wear column for tool 3, under the diameter column. It then uses the numbers you have entered for that tool to compensate for the tool's actual diameter.

G40 cancels cutter comp.

[Gabe Newell]

Hey, Jeff.

I assume you are using SolidWorks for your modeling if you are using CamWorks?

I have a Haas mini-mill and used to use CamWorks before switching to HSMWorks.

If that's the case, why not take the base sketch of the inlay pocket and offset it by .001" inwards and then save it as a different part?

Yes, you'd have two programs, but it's probably a lot less guesswork.

Gabe

By the way, I still have and love the Triton you made for me.

[Pondo]

Originally Posted by kutter % O0001 N1 G00 G90 G49 G20 Z0 <--basic header reset N2 T03 M06 (3/32 2 FLUTE HSS EM) <--change to T3 N3 S6000 M03 <--Spindle on Clockwise @6K N4 G00 G54 X3.0238 Y.4681 S6000 M03 <--Picks up G54 offset (and redundant spindle on) N5 G43 H03 Z.1 M09 <--Moves to Z.1and picks up Height offset for T3 (M9 is coolant off) N6 G01 Z-.125 F2. <--Feed to Z -.125 (G01= feed; G00=Rapid N7 G41 D23 X3.0424 Y.4606 <--Here is the dia comp start. Like I thought, the tool description in the CAM program has the dia as 23. Change it in Camworks. It should read D03 to pick up the T3 diameter offset. N8 X4.3085 Y.4197 F10. N9 G02 Y.1284 R.1457 N10 G01 X1.7863 Y.0468 N11 G02 X1.7029 Y.0699 R.1449 N12 G03 X1.4887 Y.063 R.188 N13 G02 X1.407 Y.0345 R.1448 N14 G01 X.307 Y-.0011 N15 G02 X.1762 Y.0725 R.1449 N16 G01 X.1027 Y.2028 N17 G02 Y.3452 R.1448 N18 G01 X.1762 Y.4755 N19 G02 X.307 Y.5491 R.1449 N20 G01 X1.407 Y.5135 N21 G02 X1.4887 Y.485 R.1449 N22 G03 X1.7029 Y.4781 R.188 N23 G02 X1.7863 Y.5013 R.1449 N24 G01 X3.0524 Y.4603 N25 G40 X3.0714 Y.4666 F2. <--Cancels the cutter comp N26 G00 Z.1 N27 X3.0216 Y1.0335 N28 G01 Z-.125 F2. N29 G41 D23 X3.0402 Y1.0261 N30 X4.3062 Y.9851 F10. N31 G02 Y.6938 R.1457 N32 G01 X1.7841 Y.6122 N33 G02 X1.7007 Y.6354 R.1448 N34 G03 X1.4864 Y.6285 R.188 N35 G02 X1.4047 Y.6 R.1449 N36 G01 X.3048 Y.5644 N37 G02 X.1739 Y.638 R.1449 N38 G01 X.1004 Y.7683 N39 G02 Y.9107 R.1448 N40 G01 X.1739 Y1.041 N41 G02 X.3048 Y1.1146 R.1448 N42 G01 X1.4047 Y1.079 N43 G02 X1.4864 Y1.0505 R.1449 N44 G03 X1.7007 Y1.0436 R.188 N45 G02 X1.7841 Y1.0667 R.1449 N46 G01 X3.0501 Y1.0258 N47 G40 X3.0692 Y1.032 F2. N48 G00 Z.1 N49 G91 G28 Z0 <--Moves to home reference point in Z N50 G28 X0 Y0 <--<--Moves to home reference point in X and Y N51 M30 %

It depends on how your machine is set up whether or not it reads the diameter or a radius comp. If you input -.001 in the controller it will either make the pocket +.001 bigger if it is set up as a diameter or +.002 if it is set up as a radius comp. I would try half of what you want it to take and see. My Minimill came set up from the factory as diameter comp but I changed it to Radius. Every mill I've ever worked on - Fanuc, Tiger, OKK, Haas, Fadal - has been set up to read the comp as the tool radius. In the CAM program I use, the comp is called CRC - Cutter Radius Comp.
As far as the program above, it should work fine with a couple thou comp as soon as it is changed to D03 and a comp value is put in the tool page in the controller.

[kutter]

Thanks for the info. Things are starting to clear up a bit. I'm wondering if I shouldn’t have posted this in the Camworks section. But it appears there is a setting on the machine that I need to change. i.e.: cutter comp to radius.

And thanks Pondo for the line by line help.
And thanks Mr. Newell, you are correct regarding the software. The process you described about offsetting the part and saving is what i have used in the past, and certainly works. I was just hoping to maximize the potential of the software and machine. I've never had any formal training, the machine just showed up on a truck and I endeavored from there. Always wondered about all those setting and wondering all the while if I was using everything appropriately. In that vain I have a few other questions beside my original one. I’m glad you like the knife.

But back to the first...
In camworks I find a couple place’s that I’ve never fiddled with.
In CW tool page there is a setting called "OUTPUT Through"= Tip, and this has always been selected. Option is "Center"

On another CW page “NC”, is CNC finish para’s, Options are:
CNC Comp. off/on
Toolpath center, with or without comp

In the below example, and I’ve double-checked this in CW, comp is set to Tip, with comp on, with toolpath center with comp.

What CW is showing on line N7, as D23, I can’t figure out. And can find no reference in CW regarding this setting (D23). CW says the tool is .093"

I programmed these inlays as simple bosses; all comp’d as above. Which begs the question as to why on line N23 it was cancelled before the second inlay was cut.
Although both inlays seemed to be the same size and they worked fine. Just don’t know why…
%
O0001
N1 G00 G90 G49 G20 Z0 <--basic header reset
N2 T03 M06 (3/32 2 FLUTE HSS EM) <--change to T3
N3 S6000 M03 <--Spindle on Clockwise @6K
N4 G00 G54 X3.0238 Y.4681 S6000 M03 <--Picks up G54 offset (and redundant spindle on)
N5 G43 H03 Z.1 M09 <--Moves to Z.1and picks up Height offset for T3 (M9 is coolant off)
N6 G01 Z-.125 F2. <--Feed to Z -.125 (G01= feed; G00=Rapid
N7 G41 D23 X3.0424 Y.4606 <--Here is the dia comp start. Like I thought, the tool description in the CAM program has the dia as 23. Change it in Camworks. It should read D03 to pick up the T3 diameter offset. I can find any reference in CW as to Dia. except .093”
N8 X4.3085 Y.4197 F10.
N9 G02 Y.1284 R.1457
N10 G01 X1.7863 Y.0468
N11 G02 X1.7029 Y.0699 R.1449
N12 G03 X1.4887 Y.063 R.188
N13 G02 X1.407 Y.0345 R.1448
N14 G01 X.307 Y-.0011
N15 G02 X.1762 Y.0725 R.1449
N16 G01 X.1027 Y.2028
N17 G02 Y.3452 R.1448
N18 G01 X.1762 Y.4755
N19 G02 X.307 Y.5491 R.1449
N20 G01 X1.407 Y.5135
N21 G02 X1.4887 Y.485 R.1449
N22 G03 X1.7029 Y.4781 R.188
N23 G02 X1.7863 Y.5013 R.1449
N24 G01 X3.0524 Y.4603
N25 G40 X3.0714 Y.4666 F2. <--Cancels the cutter comp
N26 G00 Z.1
N27 X3.0216 Y1.0335
N28 G01 Z-.125 F2.
N29 G41 D23 X3.0402 Y1.0261
N30 X4.3062 Y.9851 F10.
N31 G02 Y.6938 R.1457
N32 G01 X1.7841 Y.6122
N33 G02 X1.7007 Y.6354 R.1448
N34 G03 X1.4864 Y.6285 R.188
N35 G02 X1.4047 Y.6 R.1449
N36 G01 X.3048 Y.5644
N37 G02 X.1739 Y.638 R.1449
N38 G01 X.1004 Y.7683
N39 G02 Y.9107 R.1448
N40 G01 X.1739 Y1.041
N41 G02 X.3048 Y1.1146 R.1448
N42 G01 X1.4047 Y1.079
N43 G02 X1.4864 Y1.0505 R.1449
N44 G03 X1.7007 Y1.0436 R.188
N45 G02 X1.7841 Y1.0667 R.1449
N46 G01 X3.0501 Y1.0258
N47 G40 X3.0692 Y1.032 F2.
N48 G00 Z.1
N49 G91 G28 Z0 <--Moves to home reference point in Z
N50 G28 X0 Y0 <--<--Moves to home reference point in X and Y
N51 M30
%

All that said I believe I understand what to do to shrink or swell a part even if i have to manually edit the code. Just not sure how the stream line it so that isn't necessary. And i really like to understand WHY something works or doesn't.

Some other questions. I checked the machine and here is what i have in the setting page.

#33 cord system = yasnac
#40 tool offset measure = Dia.
#43 cut comp type = A
#58 cut comp = fanuc
#44 Min F in Rad CC% = 50
#85 Max corner rounding = +.005"

Under parameters
Door stop SP =0. If i change to 1 will I be able to stop over riding the door hold every time I use the machine?

As i mentioned, I've never changed anything on the machine. So I apologize if these seem like silly questions, i just don't want to screw it up...

Thanks for the info. Things are starting to clear up a bit. I'm wondering if I shouldn’t have posted this in the Camworks section. But it appears there is a setting on the machine that I need to change. i.e.: cutter comp to radius.

And thanks Pondo for the line by line help.
And thanks Mr. Newell, you are correct regarding the software. The process you described about offsetting the part and saving is what i have used in the past, and certainly works. I was just hoping to maximize the potential of the software and machine. I've never had any formal training, the machine just showed up on a truck and I endeavored from there. Always wondered about all those setting and wondering all the while if I was using everything appropriately. In that vain I have a few other questions beside my original one. I’m glad you like the knife.

But back to the first...
In camworks I find a couple place’s that I’ve never fiddled with.
In CW tool page there is a setting called "OUTPUT Through"= Tip, and this has always been selected. Option is "Center"

On another CW page “NC”, is CNC finish para’s, Options are:
CNC Comp. off/on
Toolpath center, with or without comp

In the below example, and I’ve double-checked this in CW, comp is set to Tip, with comp on, with toolpath center with comp.

Why CW shown on line N7 as D23 I can’t figure out. And can find no reference in CW regarding this setting (D23).

I programmed these inlays as simple bosses; all comp’d as above. Which begs the question as to why on line N23 it was cancelled before the second inlay was cut.
Although both inlays seemed to be the same size and they worked fine. Just don’t know why…
%
O0001
N1 G00 G90 G49 G20 Z0 <--basic header reset
N2 T03 M06 (3/32 2 FLUTE HSS EM) <--change to T3
N3 S6000 M03 <--Spindle on Clockwise @6K
N4 G00 G54 X3.0238 Y.4681 S6000 M03 <--Picks up G54 offset (and redundant spindle on)
N5 G43 H03 Z.1 M09 <--Moves to Z.1and picks up Height offset for T3 (M9 is coolant off)
N6 G01 Z-.125 F2. <--Feed to Z -.125 (G01= feed; G00=Rapid
N7 G41 D23 X3.0424 Y.4606 <--Here is the dia comp start. Like I thought, the tool description in the CAM program has the dia as 23. Change it in Camworks. It should read D03 to pick up the T3 diameter offset. I can find no reference in CW as to Dia. except .093”
N8 X4.3085 Y.4197 F10.
N9 G02 Y.1284 R.1457
N10 G01 X1.7863 Y.0468
N11 G02 X1.7029 Y.0699 R.1449
N12 G03 X1.4887 Y.063 R.188
N13 G02 X1.407 Y.0345 R.1448
N14 G01 X.307 Y-.0011
N15 G02 X.1762 Y.0725 R.1449
N16 G01 X.1027 Y.2028
N17 G02 Y.3452 R.1448
N18 G01 X.1762 Y.4755
N19 G02 X.307 Y.5491 R.1449
N20 G01 X1.407 Y.5135
N21 G02 X1.4887 Y.485 R.1449
N22 G03 X1.7029 Y.4781 R.188
N23 G02 X1.7863 Y.5013 R.1449
N24 G01 X3.0524 Y.4603
N25 G40 X3.0714 Y.4666 F2. <--Cancels the cutter comp
N26 G00 Z.1
N27 X3.0216 Y1.0335
N28 G01 Z-.125 F2.
N29 G41 D23 X3.0402 Y1.0261
N30 X4.3062 Y.9851 F10.
N31 G02 Y.6938 R.1457
N32 G01 X1.7841 Y.6122
N33 G02 X1.7007 Y.6354 R.1448
N34 G03 X1.4864 Y.6285 R.188
N35 G02 X1.4047 Y.6 R.1449
N36 G01 X.3048 Y.5644
N37 G02 X.1739 Y.638 R.1449
N38 G01 X.1004 Y.7683
N39 G02 Y.9107 R.1448
N40 G01 X.1739 Y1.041
N41 G02 X.3048 Y1.1146 R.1448
N42 G01 X1.4047 Y1.079
N43 G02 X1.4864 Y1.0505 R.1449
N44 G03 X1.7007 Y1.0436 R.188
N45 G02 X1.7841 Y1.0667 R.1449
N46 G01 X3.0501 Y1.0258
N47 G40 X3.0692 Y1.032 F2.
N48 G00 Z.1
N49 G91 G28 Z0 <--Moves to home reference point in Z
N50 G28 X0 Y0 <--<--Moves to home reference point in X and Y
N51 M30
%


Thanks again, I really appreciate all the input and help.
Mr. Newell, is HSMWorks a viable option, and not as buggy?

Regards,
Jeff

The inlays in question can be seen here if necessary.
http://customknives.net/net/manual_italia%27s.htm

[Pondo]

Jeff,
The D setting for the tool should be in the tool description. I don't know where that is in Camworks, I never used that program. In every CAM program I've used you either right click on the tool and then on "edit tool" or something similar or you double click on the icon of the tool.

The cutter comp cancel (G40) is needed at the end of each individual toolpath. If you look at line 29 it turns it on again for the other path, and then off again on line 47.

The setting to change to a radius offset is 40. Yours is set to diameter. What that means is that if you want your pocket to cut .002 bigger, then you set the tool dia to -.002. If that setting is "radius", then you would set the tool rad to -.001.
Think of it like this to make it simple - you are telling the machine that the mill is smaller, so it adjusts the toolpath to match. It is used for both fine tuning the size of features and for utilizing resharpened tools.
That's what machinists use to cut critical features to exact sizes. If I have to fit a pocket to an insert, it needs to be within +.0002 to +.0005 of the insert. I'll set the tool radius offset to .001 and run the tool. Then adjust the diameter -.0001 or -.0002 at a time until the insert slips in. Adjust-run-check, adjust-run-check, until it's exactly right.
For resharps, it's necessary to comp in the mill. For instance, if I have a 1/2" resharp mill that mics up at .470, I need to set my rad comp on the settings page to -.015. For your current diameter comp, you would set it as -.030 and the controller would know to move the toolpath out by .015.
The D23 in your program will work, but what it's doing is reading the diameter offset for tool 23 on your offset page. So you can either edit it to read D3 and pick up the T3 offset, or adjust the T23 offset to get what you want.

As far as the door stop parameter - I would really like it if it didn't have to be overridden every time I turn on the machine too. As far as I've found there is no way to do it. I've worked on Haas mills from 1996 and they have the setting 51 override too. It's a liability issue with Haas, so there is no way around it. If there is one I'd change it in a second on my mill.

Setting 85 is the max the machine will overtravel in a high feed corner. It can be set all the way down to 0, but it causes the machine to run slower as it then sees each change in direction as an exact stop. The smaller the value the more accurate, but slower, the machine runs. The setting right below it, 191, uses several settings and parameters including setting 85 to set up how fast Vs. accurate the machine runs. I run mine at medium and setting 85 at .003. I do a lot of 3D surfacing in aluminum @200IPM+ and it easily repeats within .001 all day.