[gbpacker]

i am learning and usually when i set up machines i know the distance from the home position to the table so that i can calculate the z fixture offset. i have been working with a new machine and dont know how to find the distance to the table. if someone could tell me how to find this distance or a new way to set the z fixture offsets it would be appreciated.

[Get lucky]

I would use a standard of some sort.

Bring the machine to home, set the machine positions to zero. then feed the machine down past the standard. Feed the z up until the the standard slides between the spindle nose and the table. Now take the length of the standard and the length in the position page. Add the two numbers together that should give you the length from the table to th spindle nose.

Kyle

[masonbcaldwell4]

As far as fixture offsets are concerned, I mount a travel indicator in the spindle, zero it on the table, and record the number in Z from the screen. Then, zero the indicator on top of the part and record the Z value. (make sure you use the same zero on the indicator). on my machine, the first value is negative, so what I do is disregard the negative sign and add the 2 numbers together as positives. the result is your Z fixture offset. I also set all my tools from the same spot on the table as where I zero the indicator, so there is less room for error. hope this helps.

[jlembas]

I used this technique today in hopes of speeding up my setup times. I set all the tools to the table. Then I measured the z offset from the table to each fixture. Everything makes sense at this point.

The only problem is that when I run a program, the z axis goes UP from the CS position and over-travels. If I remove the z offset in the fixture table the machine doesn't over-travel. I know there is a setting in mastercam that probably prevents the spindle from going up on the start of a program?? Anyone else have this problem? I'll be looking into the first few lines of the the post tomorrow.

[FastFieros]

I am the last person that should try to explain this... I have yet to get my Z offsets perfect like a pro would...

I use MasterCam too however.

your problem is in the offset number however you are giving Z. Negative the Z goes from CS Zero to table. Positive and it goes UP to over travel.

From CS, which is also your ZERO for part home I hope. Thats the way the most people on here recommend.

Now, going to the table with Z, the sign is Negative.

If you get to lets say -10.00 to the standard, and the standard is 4.00, you are -14.00 from spindle to table top.

Now if you take that -14.00 and enter it to the Z offsets for lets say E1, then every time you call E1 in the program it will set that spindle right on the table. ( NO TOOL YET )

Now put a tool in the spindle and you go to the table with your 4 inch standard again, and now you touch off the standard with the tool. Lets say it is -5.00 on the screen, the standard is 4.00 .. you add the numbers as both positive 5+4 = 9 .. it is -9 from CS ( Zero ) to table ...

Now if you go to E2 lets say so E1 is still there as reference and you enter -9.00 as Z offset, every time you call E2 in the program you are going to be tool on table but not cutting.

Now in mastercam you have put in Depth as -1.00 , and now you are cutting your table 1 inch deep.. NOT a good idea however. Step away from the controls.. you are fired.

OK, now you want a vise on the table. Vise is 6 inches tall lets say. Its on the table. remember E2 was -9.00 from tool tip to table. -6.00 .. now the offset in E2 needs to be -3.00... OK, some crazy math ... I hate math..
At this point however the tool tip is right on top of the vise cutting air.

Back to Mastercam program, we have -1.00 as Depth, lets hope we are cutting a circle maybe in the vise jaws. the boss is happy and you are not fired this time.

Thats the way I am going to start doing it so my tools are measured from the table, and not the top of parts.

Now if someone posts I should remove all this so it does not confuse someone, I will. Really just trying to see if I even understand it correctly on using the table surface and not the top of part surface all the time.

You have to really watch that E1 E2 calling with the Z offsets. You can have nothing in the X Y but need the Z for tool offsets.

[SBC Cycle]

I've been using Z offsets in the fixture table for a long time. The easy way to think of it is that it's like using the Mass Modify utilities for the tool lengths. If your Z fixture offset is +2.875, all your tool lengths will effectively be offset +2.875 (tool lengths are always negative so this makes your tool "shorter") when this E offset is in effect.

I never had the problem with the tool going up (Z+) past the CS until I started using CAD/CAM. So the first place I started looking was what was being put in the code differently from my hand programs. Through trial and error, I finally figured out its was the G49 "safe" code in the opening lines my CAM system was sticking in there. I can't explain why, because to be honest I don't really understand but I have had no more problems like this since I removed it.

FF is right, the Z offset can be real tricky, especially if you use multiple E's. Once you get the hang of it you'll never go back to doing it any other way.

I use Format 2, here are my program starts, tool changes, and end of file code.

O1
G20
G0 G17 G40 G80 G90
T1 M6
S2000 M3
G90 E1 X-.28 Y.28 (The G90 is redundant, not necassary but I like it)
G43 Z2.5 H1 (The G43 is also redundant and not necassary, you must use the H though)
M8 D1 (I call the D so that it will show on the screen, the control has a habit of blanking it out on the screen)
Z.25
G1 Z-1. F35.
......
CUTTING
......
G0 Z0.25
Z2.5
M9
M5
G53 Z0 (G53 is changing the coordinate system back to machine coordinates, all H's are cancelled on this line. Z returns to CS position)
M1
T2 M6
S1500 M3
G90 E1 X-.15 Y0.15
G43 Z2.5 H2
M8 D2
Z0.25
....
CUTTING
....
G0 Z0.25
Z2.5
M9
M5
G53 Z0
X0 Y0 E48 (This is sort of my own thing, I find a spot where I want the table to be for part change and set it at E48, same as Y10. E0)
T2 M6 (This is important too, this forces the Z to the tool change position and keeps it there, otherwise you get a Z move when the M30 is read)
M30

[DareBee]

interesting.

I have never used a tool change call at the end of my program to keep the Z from moving and have never had my Z move when it reads an M30.

[SBC Cycle]

interesting.

I have never used a tool change call at the end of my program to keep the Z from moving and have never had my Z move when it reads an M30.

I don't know why it does that, any insight would be nice.

Come to think of it, I haven't tried to eliminate it since I started using the G53 Z0 call.

[jlembas]

Thanks guys. I think the G49 call is my culprit too. I'm going to remove it and see what happens.

[jlembas]

Well, G49 was not the problem. Still searching.

[SBC Cycle]

Bummer. Can you post a sample part file where this happens? Preferrably one with a tool change in it. Does this happen at Auto cycle start or when you start in the middle of a program?

[SBC Cycle]

interesting.

I have never used a tool change call at the end of my program to keep the Z from moving and have never had my Z move when it reads an M30.

I tried to eliminate the tool change call at the very end. As soon as it hits the M30, the Z tries to travel +12 inches or something above the tool change position (CS). Would love to know why this happens.

[jlembas]

My problem is happening with Auto Cycle Start. I have narrowed it down to these lines:

N100 O1020 ( PF2_FORK_JAWS_OP1 )
N110 ( CREATED ON 09-02-09 AT 12:43 PM )
N120 ( T2 | 1/2 FLAT ENDMILL POWDER | H2 )
N130 G20
N140 G0 G17 G40 G49 G80 G90 H0 E0 Z0
N150 T2 M6
N160 A-0.
N170 G0 G90 S500 M3 E1 ...........

[jlembas]

Got it!! Well so far so good anyway. I post back if I discover any issues.

Changed from format 1 to format 2. Apparently format 1 moves Z whenever an offset is called out. Format 2 will only move when told.