tool offsets work offsets driving me nuts..what am i doing wrong?

Deleted info

Figured it out......LOL

How do you delete a post completely?

It’s driving me nuts too. Care to share what you’ve learned? Or anyone else???

LOL

I do the tool offset by using the spindle face on a block, then bring tool to the same block, tool offset is positive.

Work offsets: set x and y and z but on my 6m i have to look at position screen to enter values.

I can get the spindle to go to the work offset point but have to add x0 y0 Z-1.0

A plain g54 in the code does nothing.

However when the program goes to G43 H01 , Z goes positive (up) the tool offset length, I dont know why????

MwTech Inc said:

I can get the spindle to go to the work offset point but have to add x0 y0 Z-1.0



However when the program goes to G43 H01 , Z goes positive (up) the tool offset length, I dont know why????

Click to expand...

Where have you set G54? It should be a negative value from machine zero. (Meaning at the tool change position absolute Z reads some positive value)
If not, then G43 will try to raise the tool the positive offset amount usually leading to a Z axis overtravel.

well thats the weird thing, what i cant figure out...

g54 is -12.xxx I think x is 7.xxx ...y -8.xxx

My tool change is at 0.00 . I say that because I zero the machine on start up and if i use the command section i can change tools. ATC works fine.

tool offset for t1 is 4.250 ...so hits line g43 ,up it goes 4.250

Does this have anything to do with g90/g91 ??

Do i have g90/g91 in the wrong place??

Note: I am "copying" the beginning code from a program that was used on this machine years ago. I assume it worked??
I'll post the code tomorrow, 12 am here now...lol and this is my first CNC, so learning......

What happens if the G43 line says G90 G43 H01 Z1. ?

Van
Not sure if I put that in that way ....I will tomorrow

MwTech Inc said:

well thats the weird thing, what i cant figure out...

g54 is -12.xxx I think x is 7.xxx ...y -8.xxx

My tool change is at 0.00 . I say that because I zero the machine on start up and if i use the command section i can change tools. ATC works fine.

tool offset for t1 is 4.250 ...so hits line g43 ,up it goes 4.250

Does this have anything to do with g90/g91 ??

Do i have g90/g91 in the wrong place??

Note: I am "copying" the beginning code from a program that was used on this machine years ago. I assume it worked??
I'll post the code tomorrow, 12 am here now...lol and this is my first CNC, so learning......

Click to expand...

Hello MwTech Inc,
In your first Post you say that you bring the spindle face down to a block (Zeroing the Z Relative Position Readout I suspect - or you should be) and then do the same for the tool you're getting the Tool Length Offset for. In this case the Tool Offset will be from the Tip of the Cutting Tool to the Gauge Line (Spindle Face) of the Tool Holder and as you have correctly stated, will be a Positive Number.

To set the Work Shift in Z for a particular Work-piece, you need to find the distance from the face of the Spindle (given that is the datum you're using to set the Tool Length Offsets) to the Z Zero of the Work-piece. When setting up for a new job, there is likely to be material to be removed from the Top Surface to get to Z Zero and this needs to be taken into consideration when calculating the Z Work-shift value; however, for the sake of this example, the Top Surface of the Work-piece will be Z Zero.

The following can be automated using as simple User Macro Program, or there may be a Measure Feature built into the control to calculate the Z Work-Shift. However, for the sake of explaining the value that needs to be registered as the Z Work-shift, following is the basic, manual method of calculating the Z Work-shift.

1. Load a tool into the spindle that has had its Tool Length correctly established and registered under the Tool Number's corresponding Offset Number; lets say for argument sake that it's Tool Number "1" and it's Tool Length Offset should be registered in Offset Number "1". You look up the Offset Value in Offset Registry "1" and find that its 4.5".

2. Move the Spindle Tool to touch the top surface of the Work-piece and for the sake of this example, the Machine Coordinate System value being displayed for Z is -12.0". This represents the air gap between the tip of the Tool and the top surface of the Work-piece when the Z axis is at the Z Reference Return Position and Machine Coordinate System value is Z0.0000.

3. As what you need is the air gap between the Face of the Spindle and Z Zero of the Work-piece, when the Z Axis is at Reference Return, you need to combine the Tool Length Offset Value of the Tool being used, with the value of the Z Machine Coordinate System value when the tool is touching the top surface of the Work-piece.

4. Because the Tool Offset is a Plus Value and the Z Machine Coordinate System value is a Minus Value, you have to subtract the Plus Value from the Minus Z Machine Coordinate System value, as shown following:

ZWS = -12.0 -(4.5)
ZWS = -16.5

As the Z Work-shift will always be a Negative value, you will soon realize that an easier method if using a calculator, is to take the Absolute Value of the Z Machine Coordinate System value (convert this Minus Value to a Plus Value) and then add the Tool Length Offset value of the Spindle Tool to the Absolute Value of the Z Machine Coordinate System value.

ZWS = 12.0 + 4.5
ZWS = 16.5

Because the air gap between the Face of the Spindle and the Z Zero of the Work-piece, when the Z Axis is at Reference Return, is always going to be a Negative Value, simply convert the answer immediately above to a Negative Value and that's the value that's registered in the Z registry of whatever Work-shift number you're using.

When applying the Tool Offset (depending on parameter setting), you normally have to move the Tool to a Z coordinate when the Tool Offset is being called. However, you first need to specify the Work-shift number to make it active. Following is a common method used:

G91 G28 Z0.0
G28 X0.0 Y0.0
T01 M06
S2000 M03
G90 G00 G54 X0.0 Y0.0 (MAKE G54 WORK-SHIFT ACTIVE AND MOVE TO X0.0 Y0.0)
G43 Z0.5 H01 M08

With the last Block above, without specifying Z0.5 (or whatever Z Value you need to take the tool to in Z), the Z axis would move (try and move) 4.5" in a Plus direction and invariably over-travel. What the above G43 line is commanding is as follows:

Move the Spindle Face through the Z Work-shift value of -16.5", less the Z0.5 specified in the G43 Block. However, there is a Tool in the Spindle and therefore, it's Tool Length Offset is applied in the Plus direction that's been registered in the Tool Length Offset Registry. Accordingly, the total amount moved in the Z Axis by the G43 Z0.5 H01 M08 will be -16.4 + 4.5 + 0.5 = -11.5"

Regards,

Bill

Bill
Thanks for the post....I have read a couple times......I think i see my error/s...
Have an appointment I must go to so I'll digest this on my return.

Finally .....it works.

my errors were: not "adding" the tool offset value into work offset Z.......... and not inserting any "Z" value in the g43 line

Bill

Ok attached a picture of the program...

All is good until it hits the first g01

instead of going down .500 it goes 1.000????

Z does stop .500 above the workpiece. in the g43 line so im going an additional .500 after it reaches z workpiece zero

if i change the amount it still goes down two to three times the distance entered....

Running the second G01, it does move the 2.0 exactly

What up with Z being so stupid???

MwTech Inc said:

Ok attached a picture of the program...

All is good until it hits the first g01

instead of going down .500 it goes 1.000????

Z does stop .500 above the workpiece. in the g43 line so im going an additional .500 after it reaches z workpiece zero

if i change the amount it still goes down two to three times the distance entered....

Running the second G01, it does move the 2.0 exactly

What up with Z being so stupid???

Click to expand...

MwTech Inc,
Are you saying that it moves down 1.000" from where the tool stops at Z0.5 in the G43 Block, or are you saying that the tool goes to Z-1.000. If the former, that what it should do. In Absolute Mode (G90), starting at Z0.5 and going to Z-0.5, the Z axis will travel Z-1.000.

If you wanted the tool to move -0.500 from Z0.500 in G90 Mode, then your command line would be:

G01 Z0.0 F10.0

Regards,

Bill

Back to square one..

You are confusing absolute and incremental coordinates. G90 and G91,
WHICH YOU ***SHOULD** HAVE IN YOUR SAFETY BLOCK!!!!

Absolute. Every point in the box (machine travel) has a specific point assigned to it.
And you program to go to that point.

Incremental.. Where you are is ALWAYS 0,0,0 and you program the move based on that.

At Z.500, in absolute, I would 100% expect the move to the coordinate Z-.500, to be a
one inch move.

Just take some more time, slow down, and get your head wrapped around it.. Its not
easy at first, but then it just becomes second nature.

OK i get it.

When you are doing a g54 thing z is always referenced off the "Z0" of the work piece...right?

Went back and did your line of code all works

"""Are you saying that it moves down 1.000" from where the tool stops at Z0.5 in the G43 Block,"" Yes

So this g90/91 thing has me a bit confused i understand 90 means to work off machine cord and 91 means to go to the next spot from where you are...

So...i guess im just not sure when you use either one in the program, course all im doing right now is copying stuff from folks....LOL

Sems you start with 90 to get the machine to "zero" then you switch to 91 to make the moves???

Bobw post came in while writing...I think im getting a better grasp ....

So are my first two lines correct?? Do i have a safety line???

Bill
thks again

The first two lines in your program are pretty universal safety lines.

What I don't see is a tool named: T1(or T0101, T101, etc) before the G43 line. May not make any difference, but it just doesn't look right to me.

I just havent put the tool thing in this trial program...so just using tool 1 in the spindle .

Once i get my holders from Maritool i'll setup the ATC

G43 line puts you at absolute Z0.5
G01 line puts you at absolute Z-0.5
Difference is 1.0" in Z negative direction
Machine is doing what you programmed

MwTech Inc said:

OK i get it.

When you are doing a g54 thing z is always referenced off the "Z0" of the work piece...right?

Went back and did your line of code all works

"""Are you saying that it moves down 1.000" from where the tool stops at Z0.5 in the G43 Block,"" Yes

So this g90/91 thing has me a bit confused i understand 90 means to work off machine cord and 91 means to go to the next spot from where you are...

So...i guess im just not sure when you use either one in the program, course all im doing right now is copying stuff from folks....LOL

Sems you start with 90 to get the machine to "zero" then you switch to 91 to make the moves???

Bobw post came in while writing...I think im getting a better grasp ....

So are my first two lines correct?? Do i have a safety line???

Bill
thks again

Click to expand...

You’re really not going to want to use G91 (Incremental Positioning) at all other than the G28 lines when you send the spindle or table home. Everything else should be in G90 (Absolute Positioning), ideally. There are cases where you may want to do it incrementally but in most cases it’s not great and most CAM doesn’t output incremental motion either.

You do have a safety line at the top, you’re putting your machine in Rapid Motion (G0), Absolute Positioning (G90), XY Plane Selection (G17) and canceling any canned cycles (G80). These are preferred incase you stop in the middle of a program and restart. Ensures you don’t start in the middle of a canned cycle or different plane selection or remain in incremental positioning. You can have more in there that cancel tool offsets/etc but some controls don’t like that for whatever reason. The four codes you have are pretty standard. Next line you have is sending the spindle home. Good to have that there.

ok, well it sort of seems backwards....

It thought that absolute meant that everything was referenced off of axis home positions and incremental was moving from spot to spot once you got going.
Bu i see i was wrong in that assumption

ok wait...did the light bulb go off...lol.......... does the g54 xo yo zo become the "new" home position and therefore you do absolute moves from that zero reference??

dis i finally get it????

Yep.