tool blending program

[Rick46]

does anyone use a program or macro to blend tools off to there "Z" zero surface. I know on some of the machines I run when I use the touch off probe it only gets us with in a .001 or .002. then I have to manually hand wheel the tool down till it blends to the surface I want to be touched off on and adjust my tool offset accordingly. looking for a program or macro to run out of memory that will run continuously while I adjust my offset until It just blends to the surface I want to be touched off on..

 

thanks in advance.

[Compaq007]

Here is a suggestion:

 

Test the tools.

 

Before starting the job but after touching off the tools, mill a small .005 deep flat on the corner of the material (scrap piece preferably same material) removing the same amount of material. Do this for every tool and check the top of each flat with the indicator to see the difference. This should get you within tenths in the Z direction.

If needed you can mill side checks at 90 degrees and also at 45 degrees for ball end mills. That should give you an idea about the tool runout in case of oversize cutting..

 

Good luck

[Redfire427]

If you are using a touch off probe that only gets you to .001 or .002", then you either have a very poor quality machine, or a very badly calibrated probe. Try using an inexpensive tool setter and I'm sure you could get accuracy to less than .0005", unless, you are using a Haas, in which case, there is no cure.

 

Carmen

[Rick46]

When u deal with thermal expansion of the spindle the probe only is so accurate hence the need of a blending program

[The Cathedral]

Super easy macro to make. Do you want the tool to move continuously and you stop it when it makes contact and then plug in the deviation to your offset; or do you want it to make a step, plug in an offset, make another step, etc.?

[Compaq007]

Use dwell to eliminate the thermal expansion

[Rick46]

Super easy macro to make. Do you want the tool to move continuously and you stop it when it makes contact and then plug in the deviation to your offset; or do you want it to make a step, plug in an offset, make another step, etc.?

 

I guess what Im looking for is something that moves in a x or y direction going on and off the work piece surface Im trying to blend to but allowing me to change the length offset until it skims the surface. maybe something that has a optional stop at the end of each x or y move it makes to allow me to change the offset but without me having to restart the program each time a change to the offset is made. maybe runs in a loop until I get the goal im trying to achieve and then once said goal is achieved I can hit the reset button to stop the program from running. Im not sure how im going to get it to pick up the offset change every time it moves off the work piece and read the new offset that I enter before it leads back into the work piece to see if the tool is blending with the new offset change..im sure its a simple procedure but I cant picture the code I need in my head. thanks in advance..

[civiceg]

I could see doing this if each tool ran for hours. If not set tools that have to be critical off a block in .0001 step. If your tool setter is not accurate. The Renishaw tool setters I use will repeat with in .0003 or better. I check the plunger every week to make sure its still parallel to the table. I have had them move, operator hitting them etc. Set all tools at the same time when possible to avoid thermal issues. Back up tools that finish the corners of pockets .0005 and sneak up on it to avoid mismatch. The first time the Renishaw tech installed a setter at my work, we checked 10 of my tools that I set off a block in .0001 step, every tool was within .0002 of the probed value. One problem with tool setters is coming down centered with a larger diameter endmill than the plunger. The rake of the tool is giving a false reading because you are not hitting the longest from the spindle cutting edge.

 

Jobs that require minimum mismatch (trying to keep it within +/- .0002), I always warm up the machine by running above the part and re running tools that were ran first due to not being fully warm when they were ran.

[The Cathedral]

I guess what Im looking for is something that moves in a x or y direction going on and off the work piece surface Im trying to blend to but allowing me to change the length offset until it skims the surface. maybe something that has a optional stop at the end of each x or y move it makes to allow me to change the offset but without me having to restart the program each time a change to the offset is made. maybe runs in a loop until I get the goal im trying to achieve and then once said goal is achieved I can hit the reset button to stop the program from running. Im not sure how im going to get it to pick up the offset change every time it moves off the work piece and read the new offset that I enter before it leads back into the work piece to see if the tool is blending with the new offset change..im sure its a simple procedure but I cant picture the code I need in my head. thanks in advance..

 

 

I don't know what control you use; most of my experience is with Fanuc and Okuma. They work pretty similiar minus different G and M codes, and variable calls. What I would do is make a macro subprogram that can reside in your machine, and give it a number that isn't likely to be changed (in Fanuc controls you can lock out 8000 and 9000 series programs. I make my macros there and lock them). Using system variables you can pull all your numbers and have the control adjust them.

 

So lets say for example I make my macro on a Fanuc, and name it O9009.

 

In MDI I would type in a simple macro call:

G65 P9009 X1 Y0 T1

 

This calls up the macro. The X1. or Y1. would be where you tell it what direction you want it to move: in X or Y. Using a "1" would mean that's the direcion you want, a "0" means you don't want it. T obviously calls the tool you want.

 

The macro subprogram would look like this:

 

O9009(BLEND MACRO)

#500=[11000+#20] //this specifies which length offset to change

#501=0 //this is a counter

G90 //absolute mode

G43 H#20 Z.010 //this calls your length and moves .010 above the surface

N9999 //address

IF[#24 EQ 0] GOTO 8888 //X decision

N9000 //address

M01 //optional stop

G91 G1 X.1 Z-.008 F3. //ramp onto part

X.5 //move forward to make mark

X.1 Z.008 //ramp off of part

X-.7 //return to start position

Z-.0001 //move down small increment

#501=#501-.0001 //add increment to counter

GOTO 1111 //GOTO the decision process

N8888 //address

IF[#23 EQ 0] GOTO 7777 //Y decider

N8000 //same as above but in Y

M01

G91 G1 Y.1 Z-.008 F3.

Y.5

Y.1 Z.008

Y-.7

Z-.0001

#501=#501-.0001

GOTO 1111

N1111 //address

IF[#500 EQ 11001] THEN#11001=#11001+#501 //here is where it decides what tool offset you are using and adds the increment to your offset

... //not going to type them all out

IF[#500 EQ 11030] THEN#11030=#11030+#501 //your last number would correspond to your highest tool

GOTO N9999 //restart the loop

N7777 //address

#3000=1(YOU MUST SPECIFY X OR Y) //will alarm out if you didn't set X or Y to 1.

M99 //end of program

 

 

You can let the macro run in a loop until you see it touch. Once you do, you can flip on optional stop. The macro will make its additions, then stop, at which point you can reset and go home, and your tool will have the right length. This assumes that you already had your tool in a safe position to do this macro, and that you trust it enough to go down to within .010"

 

This is just a rough macro, it's up to you to finesse it the way you like. If you don't have a Fanuc I leave it up to you to find and make the necessary changes. Even if you do have a Fanuc, you'll still have to make changes depending on what model control you have.

[Rick46]

I am running a fanuc 18i-mb control on a toyoda fv1680 with a reinshaw probe and a reinshaw TS27R contact tool setting probe. I can get them synced with in about .0003 tenths but as the day goes on and the spindle warms up the part probe tends to get out of sync due to the thermal expansion. and sometimes the machine will set for a day without being run. so then when I run it first thing in the morning it should be really close to being right on but im not sure how much thermal expansion growth im working with when it heats up or how long I could run a warm up program to get it to it maximum growth before touching tools off that are critical on depths and blending to other tools..but any how thanks everyone for your input. the last time I calibrated it was when the new guy broke the stylus on the part probe and it took a good 2 hrs to get it back on center to even think about running the calibration program. I will try calibrating it when its warmed up and see if I can find a happy medium with it and the tool length setter. once I get the probe calibrated I always have to go and sync it with the tool length setter and its usually within a .002 but im just striving for 1 to 1 touch offs and tool length offsets and not within .002..

[Sticky]

You are always going to have an issue on tolerances tighter then .002" when it comes to thermal expansion. You can calibrate your part probing and tool length setting to a warm machine or a cold machine, but how warm or how cold do you use it? The type, or lack of a spindle chiller makes a world of difference in this situation;)