[Vern Smith]

I'm hoping someone can tell me when the Haas control accepts or uses a change to the tool diameter. I'm working on a vertical mill less than a year old. Yesterday I made the stupid mistake of changing a tool but forgetting to update the diameter in the offset page from zero. The software called for comp and the cutter did the predictable thing. I stopped the program, threw away the part, corrected the tool diameter and started again at the top of the program. To my surprise it did the same thing again. Just to be sure I checked the tool register to be sure the correct diameter was listed for the tool in the spindle and ran the program from the top leaving the ruined part in place. It still did not recognize the new diameter. I then called another program to active status, then called the first program to active status and ran it again. All was well.

I apologize if my terminology is not correct, I'm rather new to CNC. I looked through the manual and found lots of information on tool offsets and such but never could locate anything that described the situation I was in. There are a few guys on this site that know the Haas manuals like the back of their hands so I doubt if an explanation is far away.

Thanks for reading, Vern

[Geof]

One way you can possibly get this is if you do not use M30 at the bottom of a program...I think... or if you stopped the program part way through. This could result in the older entry being the one that was still in some memory location.

Do you have a 'safety line' at the top of the program that includes a G40 to make sure tool comp is cancelled when a program starts?

See if you can repeat what happened. I have sometimes had inexplicable things occur and have not been able to repeat them. My conclusion is that gemlins exist .

EDIT: gremlins do exist, obviously and gemlins.

[djr76]

I've never had a problem with just 'Reset'. I guess like Geof pointed out is using the G40 at the top of the program or you could just do it in MDI mode, then Reset/Edit/Mem/Curnt Comds/Cycle start.

[Vern Smith]

I'm glad to hear that an eminent authority like yourself also believes in Gremlins. They have been a constant companion of mine for 60 plus years. My CAM software always puts M30 at the end of a program but this brings up an interesting point, I did not let the program complete, rather I interrupted it when the control developed a mind of it's own and hit reset so the control never had a chance to see the M30. This was also the first time through for this program so I had used feed hold several times before coming to the comp problem. I do have G40 in my safety line.

Between the interruptions and resetting without the control seeing M30 you may have found the problem, excluding the most probable cause.....Gremlins

Vern

[Shotout]

I'm glad to hear that an eminent authority like yourself also believes in Gremlins. They have been a constant companion of mine for 60 plus years. My CAM software always puts M30 at the end of a program but this brings up an interesting point, I did not let the program complete, rather I interrupted it when the control developed a mind of it's own and hit reset so the control never had a chance to see the M30. This was also the first time through for this program so I had used feed hold several times before coming to the comp problem. I do have G40 in my safety line.

Between the interruptions and resetting without the control seeing M30 you may have found the problem, excluding the most probable cause.....Gremlins

Vern

Did you do a program restart from a specific line number after changing the value? If so this might be pertinent; we where told in school that a program restart would use the last values picked up from the offset registries. It is suppose to be part of the restart routine that unless processing an M30 or starting at the beginning of the program where the controller has to actually process the proceeding lines of code, I assume making a call to the memory address where they are stored, it just performs a true not true check on them and that this could happen.

[gar]

080108-2045 EST USA

I use a tool change routine that dynamically changes the tool diameter throughout the program. Never a problem.

Following is a portion of a program:

%
O6901
(Beta TOOL CHANGE macro subroutine 981212-1750)
     G10  G90  L12        P#7       R#18
     G80       M09
     G90       M06  T#20
     G#8       M08
     S#19      M03
     G43            H#20  D#7
  M99


O3002
(D_36_TML.CNC     Date-time created  12-15-1998   21:11:44)
(Beta prog 981205-1357  )


(**** TOOL Change to Center Drill  **** --->1    IDD13C    HAAS TL #    1  )

G65  P6901    E54   R 0.500   S 5000  T01  D01

G99 G81    F  10.0000	R   0.1000			Z  -0.0700	L0	X   2.4000	Y  -2.0000
M97    P  11
G80


(**** TOOL Change to Drill         **** --->2    IDD13D    HAAS TL #    5  )

G65  P6901    E54   R 0.250   S 4500  T05  D05

G99 G83    F  25.0000	R   0.1000	Q   0.3500	Z  -1.1000	L0	X   2.4000	Y  -2.0000
M97    P  11
G80


(**** TOOL Change to Mill Cir Rfgh Pocket **** -->3    IDM20R    HAAS TL #    8  )
(**** Tool dia is modified to get rough offset -->3    IDM20R    HAAS TL #    8  )

G65  P6901    E54   R 0.505   S 7500  T08  D08

G90       G0	X   2.4000	Y  -2.0000
							Z   0.1000
	F 20.0  
G13	K   1.6410	Q   0.3787	I   0.2535	Z  -0.3500
G13	K   1.6410	Q   0.3787	I   0.2535	Z  -0.7000
G13	K   1.6410	Q   0.3787	I   0.2535	Z  -1.0500


(**** TOOL Change to Mill Cir Fin  Circum  **** -->4    IDM20F    HAAS TL #    8  )

G65  P6901    E54   R 0.499   S 7500  T08  D08

G90       G0	X   2.4000	Y  -2.0000
							Z   0.1000
	F 20.0  
G13	I   1.6410       				Z  -0.5250
G13	I   1.6410       				Z  -1.0500


(**** TOOL Change to Mill Cir Rfgh Circum **** -->5    IDM21R    HAAS TL #    8  )
(**** Tool dia is modified to get rough offset -->5    IDM21R    HAAS TL #    8  )

G65  P6901    E54   R 0.505   S 7500  T08  D08

G90       G0	X   2.4000	Y  -2.0000
							Z   0.1000
	F 20.0  
G13	I   1.7410       				Z  -0.2235
G13	I   1.7410       				Z  -0.4470

.

[Vern Smith]

Gar,

That's very interesting. My machine currently does not have macro's enabled but will in a week or so. I'm assuming the R value is the tool diameter. If I understand your system you use the program or your CAD system to enter all the tool offsets for a particular program rather than doing it at the Haas control.

I will be installing the Renishaw probe system shortly which includes macros. Can the macro's used by the probing system be employed to handle the tool off sets as part of their tool set up templates?

Shotout,

I did not restart the program from any line number except #1.

Vern

[Geof]

It is not necessary to have macros enabled to do dynamic tool diameter changes, just use the G10 command.

G10 L12 G90 P1 R.5 sets the tool diameter entry for tool 1 at 0.5 so you can sprinkle these commands anyplace in the program.

Put in a G91 and you can increment the diameter up or down.

But my advice is don't do it this way. Should you want to change the program entries you need to find all the G10 lines and change them. This is not too difficult use the Find function in the editor but it is quicker to group all the various tool diameters in one location under different tool numbers. Haas machines have the capacity for several hundred tool diameters but rarely will you ever have more than 10, 20 or 25 tools actually in the machine depending on your toolchanger style.

As an example to use different diameters for tool 1 on a MiniMill with a ten position changer I use P1, P11, P21, P31, etc., in the G10 lines and have these all clustered right at the beginning of the program. In the program use D01, D11, D21, D31, etc.

Sometimes the diameters are the same because I am using the same tool to do different critical dimensions and I just want to be able to adjust the wear entry in a different direction; for instance if the tools is used for both an ID and an OD finish.

Sometimes the diameters are different when I am using a tool to take off a lot of material on a profile or are using a small tool for a large interpolated hole. This way I have have the profile coordinates or the hole interpolation in a subroutine and set tool comp before going to the sub. For instance if you use a P11 R1.0 for a 1/2" tool that will interpolate hole that is 1.875" ID you can write a very simple interpolation routine that uses the 0.9375 radius in the subroutine; then do G41 D11 and go the sub. The tool only moves out 0.4375, because it is using a radius value of 0.5 from the D11, and interpolates a starter hole. Cancel tool comp and return then use G41 D01 and go back to the same sub and finish the hole to size.

A similar sequence is used for profiles with the only thing to watch being concave sections. The largest 'false' D value has to be smaller than twice the radius of the smallest concave radius otherwise you get a tool to big alarm. When I have small concave radii in the profile I will have two subs, easy to do with copy/paste and for the subs called with a 'large' tool I take out the small concave radii.

[Vern Smith]

Goef,

Thanks for the detailed explanation and suggestions, give me a week or so to try to figure it out and I'll come back with some intelligent questions, maybe.

Vern

[gar]

080109-2059 EST USA

Vern:

Tool diameter/radius offsests are located at #2401-#2499 per one of my manuals.
Tool/diameter/radius wear are located at #2601-#2699.

These can be changed manually thru the table prior to execution of the program, or from within one or more programs, and the variable locations retain their last loaded value until next changed by any of the said means.

From within the program you can use the G10 command with or without macro capability to make changes from any place in the program prior to when you want to use that value. If you have macro capability you can use the assignment operation #24xx = 0.50 to load 0.5 into whatever address you need loaded. D01 is probably #2401.

Whether you set your values manually, at the beginning of the program, or distributerd thru the program is dependent upon your programming philosophy.

.

[dapoling]

I'm hoping someone can tell me when the Haas control accepts or uses a change to the tool diameter. I'm working on a vertical mill less than a year old. Yesterday I made the stupid mistake of changing a tool but forgetting to update the diameter in the offset page from zero. The software called for comp and the cutter did the predictable thing. I stopped the program, threw away the part, corrected the tool diameter and started again at the top of the program. To my surprise it did the same thing again. Just to be sure I checked the tool register to be sure the correct diameter was listed for the tool in the spindle and ran the program from the top leaving the ruined part in place. It still did not recognize the new diameter. I then called another program to active status, then called the first program to active status and ran it again. All was well.

I apologize if my terminology is not correct, I'm rather new to CNC. I looked through the manual and found lots of information on tool offsets and such but never could locate anything that described the situation I was in. There are a few guys on this site that know the Haas manuals like the back of their hands so I doubt if an explanation is far away.

Thanks for reading, Vern

Vern if you could post your code where this happen it maybe helpful as some program their tool prep and paths a little different then others.

When you stopped the cycle of from running did you hit reset.
When starting the tool cutting again did you start it from the very begining or at least calling up the tool change portion of your code.

When reading M6T1 this will also set your H and D active at this point. Some machine you can go right into a G41 with out calling up your D value as it is already active.

Dave

[Geof]

.....When reading M6T1 this will also set your H and D active at this point. Some machine you can go right into a G41 with out calling up your D value as it is already active.

Dave

Sorry, not on a Haas it will not. T1 M06 just commands a tool change to tool 1, following this you need G43 H01 to set length compensation and then G41 (or 42) D01 for diameter compensation.

When Setting 15 H & T Code Agreement is turned ON the machine checks that the H number matches the tool number so you have to use H01 for Tool 1, H02 for Tool 2, etc. For the diameter offset D you can use any number and the machine will not do a check; so it is up to the programmer to make sure the correct D value is being called for a tool.

Things are different on lathes which do make all the offset values active at a tool change so you do not need to call them later.

[Donkey Hotey]

Man, I love threads like this. I had no idea what to use G10 for and now I've got all kinds of ideas. Thanks guys!

[Geof]

Man, I love threads like this. I had no idea what to use G10 for and now I've got all kinds of ideas. Thanks guys!

Maybe now we should introduce you to G52?

[dapoling]

Vern if you could post your code where this happen it maybe helpful as some program their tool prep and paths a little different then others.

When you stopped the cycle of from running did you hit reset.
When starting the tool cutting again did you start it from the very beginning or at least calling up the tool change portion of your code.

When reading M6T1 this will also set your H and D active at this point. Some machine you can go right into a G41 with out calling up your D value as it is already active.

Dave

Excuse me the H and D is called up when the G43 used with your H offset and when you make a move with a G41 or G42 called up with your current D offset.
However the H and D are modal.

[SeymourDumore]

Ok, just so everyone is on the same page.

T1 M06 calls nothing but a toolchange. Neither length or diameter offset is read in, only Tool1 is put in spindle.

G43 by itself does nothing. It does not call the current tool's length.
Neither does G41 or G42 call the current tool's diameter by itself automatically, but it will call the previous D value!!!

So. To properly make sure that correct offsets are used, I do the following.
Each and every one of my toolchanges are done in this strict format:

(TOOL DESCRIPTION)
T1 M06
G00 G43 H01 D01

This way immediately after the tool is put in the spindle, it's appropriate offsets are also registered.
This is the only place the H and D words are called. Nowhere else within the body of the program is D called again unless there is special need to adjust some dimension and a different dia offs. is needed for that tool.

Special note: For this to work properly, you must make sure that "Program Restart" parameter is set to ON!!!

[dapoling]

In a Haas if a H or D is not placed with the appropriate G code as G43 will use the last H Offset used, this also will happen in G41 or G42 with the D value (this is not common in any other machine that I know of).

Seymour the way you are calling up your H and D work just fine, although I think this has more to do with personal choice or company policy.

Case in point I have worked with companies that used more then one D value assigned to one tool instead of correcting their program or setup to use one D value.
Thus calling up the D in the G41 D1 X1. F10. and any subsequent G41 or G42 call up also contained the same of different D value.
Either way is fine and this falls back to the ease of finding the code you are looking for while first run or editing, you will know where to look in the program with out reading the entire program.

The only time I use Program Restart is to get a tool back into a cutting path if I was just to restart at the tool change I just leave it off. This again is a personal preference or company policy.

[SeymourDumore]

That would be correct. Note that I've said D is not called again, unless due to special requirement a diff. offset is needed for the same tool.

Besides the advantage of immediate display of the proper offset, anytime you need to change a tool to a different station, you need to only change it in one place, right at the toolchange.
Find/replace works wonderful, but still does not beat a single overwrite.

[duenow]

Maybe now we should introduce you to G52?

I love G52,I run the same set of step jaws & G52 is 0 on a 1/4" plate. Run a 1/2" plate & just set G52 .250 on Z. Also handy for X & Y.

[joehernandez]

can i get the machine to ingore the d-code offset