Setting Up a Fanuc 18T

[WayneC369]

Hello All,

I've searched as far as I can on this site for the answer and cannot find it. I get six pages of results, but something seems wrong with this site as I cannot go past page two. I get a text box which says, "vBulletin Message - Sorry - no matches. Please try some different terms." when all I do is select page three. So, my apologies if I'm being redundant. Anyway onto the thread:

I recently acquired an Okuma-Howa ACT-20 lathe with a Fanuc 18T Model A control, but I think has been upgraded to Model B and I'm still getting acquainted with it. I've been reading the manuals as much as I can stand and getting NO WHERE with them fast. Damn what a mess that is!! I know it must be very simple, but I need to know how to set the tool offsets. What is step one on the control? I've read about differing locations of where to touch off the tools from - spindle nose, chuck face, part face etc. but how does that reference machine zero, or does it even matter? If I send the turret home manually the position reads X11.918 Z-3. Does this home position reference the centerline of the turret with the centerline of the spindle? So, for instance I have an on-center tool (center drill) and I dial the tool in on-center with the spindle what do I do with the X0.089 that shows on the absolute position display? Or, do I use the X-11.829 that shows up on the relative postion display? Do I plug that number into the offset page for that tool position and that's it?

This machine is well used and none if the entries in the offset table make sense to me, therefore I cannot trust them as a guide. I'm not even sure I can count on the other Fanuc control models to be close enough in function to act as a guide. It seems NO ONE is using the 18T and that in and of itself is disconcerting. Any help would be appreciated.

 

[Ox]

When your turret is HOME it likely doesn't have a tool offset loaded, and the 18 will dump your offset as soon as you hit RESET.

You say that your readout says .089 when you have your holder co-axed in.
You need to look at the BLH corner of the CRT and see what T is loaded in there at this time.
Is it T0, or is it the T that you have in place yet?

A) If it says T0, then you could likely toss .089 into the X offset for that tool and then when you call that tool in MDI or program and send it to X0, it should be right.

B) If the CRT shows that you have a tool offset loaded, and you are still showing .089 on the CRT, then you will need to lower the X value of that tool position by .089.

The 16 and newer (and maybe some other older ones?) have a nice feature that allows you to edit the offset values easier. In this case - if you need to lower the X value of this tool by .089, just highlight the X value in the tool GEOMETRY page. Key in -.089 (that is minus .089) and then hit the "+ input" key at the bottom of the CRT.

Example - .089 INPUT will result in an offset of .089.
.089 +INPUT will add .089 to the existing value in that field.
by the same token, a -.089 +INPUT will subtract .089 from the current value.

18T is a very common control, but generally not used on the penny pincher machine models.
Those will have an 0T. The old ones suck, and I have no clue about the newer ones.
Be VERY glad that you have an 18!


------------------

Think Snow Eh!
Ox

 

[WayneC369]

Thanks for your time and response, Ox.

Okay, when it wakes up it's showing T0 for the loaded tool - meaning no offset loaded (correct?). Just FYI - I'm dialing in T9. The original geometry offset had .097 entered. I have changed that to .089. I have yet to check the remaining O.C. tools, but it's on the list.

Yep, this control has that feature - "+Input".

Thank you for the reassurance on the control model.

So, I'm still hung up on the tool length offset setting. Am I understanding things correctly that I can select an arbitrary Z position and reference all tools from there? i.e. chuck face, part face, etc. Do I need to select a coordinate system BEFORE I begin setting the offsets? The manual says, "Suppose a workpiece coordinate system has been set." WTH? That tells me it really doesn't matter.

The best I can make of the manual I:

(1) Pick a tool and take a facing cut. (I choose T1.)
(2) Don't move the tool in Z but get it clear of the part in X.
(3) Measure the length of the part.
(4) Highlight the tool position you're setting.
(5) Enter the measured length in this form:"Z2.0000"
(6) Press the MEASURe soft key.

The control calculates a number and throws it into the Z position on the G offset chart. In my case it's -17.3809. Does that reference Z home?

 

[Ox]

I like G10 "Workshift" for Z.
My first Fanuc was on a Hardinge lathe (the 18T) and that is how they recommend to doo it, and I really like it.
Others don't seem to catch on so much...


To start with - go to MDI and cycle in
G10 P0 X0 Z0 and cycle it through.

10/1 odds is that you will have a Trigon in T1.
Index T1 to position and then jog it up to touch off on the Z ref plane that you want.
On a collet - it would be the face of the collet.
On a 3 jaw - you might likely use the chuck body. You could opt for the chuck jaw, but that will likely be changed frequently.

Make sure that you have T0 as the active offset.
Go back to the tool offset Geometry page and key into the Z field for T1 the value in the W column near the bottom of the screen.

Now you can repeat this for each tool if you want now, or wait ...

For X, just touch the OD of the part, go to the X field in the OFFSET page and enter the U value near the bottom of the page. Then subtract the size of the bar from that value.
Ex:
You touch off on the 1.250 bar OD at U4.500. Enter that.
Then enter -1.25 (bar OD) and hit your +INPUT and your X is real close. Hit a part and adjust from there.


Now - you have your primary tool loaded.

Now in the top of your program, you decide how far from your Z ref point that you want your PROGRAM ZERO. Lets say that you want your part to stick out 3.5" from your Z ref surface. In the header of your program you enter a line as:
G10 P0 X0 Z-3.5;
The Z will always be negative.

Now - in every program, you have this line in your header. The Z values will change, but you will have no call to change the other values. This line will always be there. You doo not hafta look it up ever again. Also - it will always be near the top of your screen every time you are at the top of your program, so you can simply look for the G10 line and know instantly how far your part is supposed to stick out.


Now face off your part with the first tool.
Ass_u_ming that you faced it off at Z0, now you can bring your other tools up to that surface and "touch them off" and simply enter the W value in your Z offset field. You are done.

Your tools will always be set. The only tools that you need to ever touch off are the ones that you change.
When you go from job to job they will all be set, and will all shift together as you go from one G10 Workshift point to the next.


I doo not have this feature on an older Mits control and I hate it. When I touch off - I always have to remember what the G54 value is and remember to subtract that value from my readout value. The Workshift is much easier.

Also - the Workshift is always on! There is not calling up the offset, and being concerned about forgetting to call it and crashing out. When you fire it up next week - the last Workshift that was read in the last program that was cycled - is still active.


------------------------

Think Snow Eh!
Ox

 

[WayneC369]

Again, many thanks, OX!

Have you been snooping around in this shop? You nailed the tool type in T1!

Not that I'm doubting you, it's just difficult for me to comprehend that it's just that simple. I plan to print this out and commit it to memory this eve by the fire. BTW - You guys can close the freezer door up there any time you like!

 

[Ox]

Header example:

O1234 (WayneC part #369)
G97, G98, G20
G10 P0 X0 Z-3.5
G0 T0 X15. (or G28 U0)
Z10.
N1 T101 (trigon)
M3 S1000
G0 X2. Z0
G1 X-.05 F5. M8
.
.
.
.
.
.
.
.
.
G0 T0 X15. Z10. M9
N2 T202


---------------
Think Snow Eh!
Ox

 

[DouglasJRizzo]

Hello All,

I've searched as far as I can on this site for the answer and cannot find it. I get six pages of results, but something seems wrong with this site as I cannot go past page two. I get a text box which says, "vBulletin Message - Sorry - no matches. Please try some different terms." when all I do is select page three. So, my apologies if I'm being redundant. Anyway onto the thread:

I recently acquired an Okuma-Howa ACT-20 lathe with a Fanuc 18T Model A control, but I think has been upgraded to Model B and I'm still getting acquainted with it. I've been reading the manuals as much as I can stand and getting NO WHERE with them fast. Damn what a mess that is!! I know it must be very simple, but I need to know how to set the tool offsets. What is step one on the control? I've read about differing locations of where to touch off the tools from - spindle nose, chuck face, part face etc. but how does that reference machine zero, or does it even matter? If I send the turret home manually the position reads X11.918 Z-3. Does this home position reference the centerline of the turret with the centerline of the spindle? So, for instance I have an on-center tool (center drill) and I dial the tool in on-center with the spindle what do I do with the X0.089 that shows on the absolute position display? Or, do I use the X-11.829 that shows up on the relative postion display? Do I plug that number into the offset page for that tool position and that's it?

This machine is well used and none if the entries in the offset table make sense to me, therefore I cannot trust them as a guide. I'm not even sure I can count on the other Fanuc control models to be close enough in function to act as a guide. It seems NO ONE is using the 18T and that in and of itself is disconcerting. Any help would be appreciated.

The Fanuc 18T is quite prevalent, and not too mysterious. As for it's version - if it's a 18T-A from the factory, it most likely still is. When they change from "A" to "B" to "C" etc, they are really making MAJOR changes to architecture.

Now onto the set up.
When you home the machine, try origin all axis. Then, by handwheel crank the X axis down until the X display for Absolute reads "0"
This most likely is the centerline (or close) to the spindle.

 

[Ox]

To start with - go to MDI and cycle in
G10 P0 X0 Z0 and cycle it through.

There is no movement in this line. It only double checks that there is not already some other Workshift value already loaded. The only change that you may see is possibly a shift in the readout position is all.

10/1 odds is that you will have a Trigon in T1.
Index T1 to position and then jog it up to touch off on the Z ref plane that you want.
On a collet - it would be the face of the collet.
On a 3 jaw - you might likely use the chuck body. You could opt for the chuck jaw, but that will likely be changed frequently.

If you touch off on a collet face - make sure that you have material in the collet and the collet chucked up to give a proper representation of where the collet will be when you are running your part.

That seems quite elementary, but just thought that maybe I should throw that out there.



---------------------

Think Snow Eh!
Ox

 

[metaltech]

If I send the turret home manually the position reads X11.918 Z-3.

WHAT position reads that value? You have ABSOLUTE (which shows where the tool tip is within the current coordinate system for that tool, moved by the programmed command), RELATIVE (which can be relative to anything, depending on where you zero it out) and MACHINE (the distance from home, accurately known as Reference Point, or zero return point, that each axis has traveled. Could be in inches or mm according to param setting.)

Does this home position reference the centerline of the turret with the centerline of the spindle? So, for instance I have an on-center tool (center drill) and I dial the tool in on-center with the spindle what do I do with the X0.089 that shows on the absolute position display? Or, do I use the X-11.829 that shows up on the relative position display?

Every machine tool builder (MTB) can set this up as they desire. Many set up the params so when an axis is at home, the MACHINE position reads 0. However, others set it up so the coordinate of the centerline of a boring bar holder will be loaded. For example, if the holder is 8" from spindle CL when the X is at home, that would be a 16" diameter that the CL of the holder is located, so they will have the MACHINE position read X16.0000. You mention "X0.089 that shows on the absolute position display". The ABSOLUTE display value will be determined by the amount in the currently active tool GEOMETRY offset, adjusted by the WEAR offset, adjusted by how far the axis is moved from home. It would also be subject to adjustment by the WORK/EXTERNAL/SHIFT offset (whatever term your control uses). However, there should NEVER be a reason to shift the X, as the spindle CL, or X0, never moves.

So, when you've indicated a drill to be on-center, what does the MACHINE position read? If it were X0.089, than one of two things are wrong. There is a param that holds the value that gets loaded into the MACHINE position when it reaches home. That value is wrong. Or, the value used to be right in the past, but the machine was wrecked, causing slippage between the motor/encoder and the ballscrew. Either the param needs to be adjusted to reflect the real position of the BB holder, or home needs to be reset. Either way, that would make the X MACHINE position read 0 when the BB holder is concentric with the spindle CL.

The offset tables themselves can be configured different ways, depending on the MTB choice. I would expect that you have a GEOMETRY OFFSET page, and a WEAR OFFSET page. In this case, the geom offset represents where the tool tip is when the axes are at home. IOW, for a turning tool tip, what diameter would it cut if it were turning a part all the way back at home? Now, if your coordinate system is set up such that you home the machine, and you have numbers OTHER THAN 0 in the MACHINE position, then the geom offset will just be the difference between the home value, and the real diameter of the tool tip. Example: At home the display reads X16.0000, but the turning tool tip is really at a 15" diameter, then it is starting too small, or too negative, by 1.000. So, the geom offset for that tool would need to be X1.000 (a positive value). This will offset or shift the tool path 1.000 larger diameter so that it matches the 16.0000 that the control thinks the tip is starting at.

As far as Z axis, you can choose where you want the 0 position, or datum, to be. It could be the spindle nose, the chuck face, the jaw face, or the face of the part. For those machines equipped with a tool presetter, it would be the face of the front button. What is critical is that whatever feature is used for the program as Z0, the tool offsets have to be set off that same surface. I would argue strongly for using the finished face of the part as 0. Doing it this way is logical, and makes it far easier to follow the program on the screen. This way, the ABSOLUTE position (the tool's position commanded by the program, including offsets) will read 0 when the tool tip is touching the finished face. If the absolute display is positive, the tip is clear of the part. If negative, it is past the face of the part. If done this way, the GEOMETRY OFFSET for Z represents how far the tool tip must travel from home to touch the face of the part. It would be a negative value, as the axis has to move in the negative direction from home to the part.

If the chuck face were used as 0, then the Z geometry offsets would represent the distance from home to the chuck face. Of course, machining in that area is detrimental to tool life, or machine life, for that matter. So, you would have to have an amount in the WORK/EXTERNAL/SHIFT offset to back the tool path away from the chuck. The amount would be the distance from the chuck face to the part face. I don't like this method, simply because if that WORK or SHIFT offset is destroyed (set back to 0), the tools will be diving into the jaws. However, the method is valid, I just think it's less tolerant of human error. Because I earn most of my living fixing machines, I tend to have great consideration for things that can go wrong and tear up machines, otherwise called failure modes. Wrecks are almost exclusively caused by human, not machine, failure modes.

 

[WayneC369]

The Fanuc 18T is quite prevalent, and not too mysterious. As for it's version - if it's a 18T-A from the factory, it most likely still is. When they change from "A" to "B" to "C" etc, they are really making MAJOR changes to architecture.

This is only my second taste of Fanuc controls. First was with an old 3000C. I made an ass_u_mption that maybe the firmware was upgraded to a Model B since "BE..." is displayed on the LCD on boot up. I didn't know lots of other things change hardware wise with model changes. Just trying to throw as much info out that I thought may be pertinent to discussion.

 

[DouglasJRizzo]

This is only my second taste of Fanuc controls. First was with an old 3000C. I made an ass_u_mption that maybe the firmware was upgraded to a Model B since "BE..." is displayed on the LCD on boot up. I didn't know lots of other things change hardware wise with model changes. Just trying to throw as much info out that I thought may be pertinent to discussion.

No worries. Just bringing what I know to the table.
At Doosan, we set the lathes so that "X0" on the absolute, is the centerline of the spindle.

 

[WayneC369]

There is no movement in this line. It only double checks that there is not already some other Workshift value already loaded. The only change that you may see is possibly a shift in the readout position is all.

Thanks for the follow through, Ox. I wondered what would happen after running this block.

If you touch off on a collet face - make sure that you have material in the collet and the collet chucked up to give a proper representation of where the collet will be when you are running your part.

That seems quite elementary, but just thought that maybe I should throw that out there.

Gotcha. I've also been figuring if there was an error in the part length one could do a work shift, or change the program at your header to correct the next part.

 

[WayneC369]

WHAT position reads that value? You have ABSOLUTE (which shows where the tool tip is within the current coordinate system for that tool, moved by the programmed command), RELATIVE (which can be relative to anything, depending on where you zero it out) and MACHINE (the distance from home, accurately known as Reference Point, or zero return point, that each axis has traveled. Could be in inches or mm according to param setting.)

These values are absolute and are displayed after manually homing both axes, i.e X11.9180" Z-3.0000"

Every machine tool builder (MTB) can set this up as they desire. Many set up the params so when an axis is at home, the MACHINE position reads 0. However, others set it up so the coordinate of the centerline of a boring bar holder will be loaded. For example, if the holder is 8" from spindle CL when the X is at home, that would be a 16" diameter that the CL of the holder is located, so they will have the MACHINE position read X16.0000. You mention "X0.089 that shows on the absolute position display". The ABSOLUTE display value will be determined by the amount in the currently active tool GEOMETRY offset, adjusted by the WEAR offset, adjusted by how far the axis is moved from home. It would also be subject to adjustment by the WORK/EXTERNAL/SHIFT offset (whatever term your control uses). However, there should NEVER be a reason to shift the X, as the spindle CL, or X0, never moves.

So, when you've indicated a drill to be on-center, what does the MACHINE position read? If it were X0.089, than one of two things are wrong. There is a param that holds the value that gets loaded into the MACHINE position when it reaches home. That value is wrong. Or, the value used to be right in the past, but the machine was wrecked, causing slippage between the motor/encoder and the ballscrew. Either the param needs to be adjusted to reflect the real position of the BB holder, or home needs to be reset. Either way, that would make the X MACHINE position read 0 when the BB holder is concentric with the spindle CL.

When I co-ax a BB holder with the spindle there is no tool offset loaded and the absolute X position reads 0.0890". I would NOT doubt the machine has been wrecked in the past given it's age. So, is resetting the home position a big deal? Off the cuff it would seem one could adjust the parameter where that home value is loaded and rock and roll. Unless this slippage resulted in some mechanical limitation of the axis. ??? I have some documentation from the MTB. I will parse it to see if they documented the value to be used when X is at home position and see if there is a discrepancy.

The offset tables themselves can be configured different ways, depending on the MTB choice. I would expect that you have a GEOMETRY OFFSET page, and a WEAR OFFSET page. In this case, the geom offset represents where the tool tip is when the axes are at home. IOW, for a turning tool tip, what diameter would it cut if it were turning a part all the way back at home? Now, if your coordinate system is set up such that you home the machine, and you have numbers OTHER THAN 0 in the MACHINE position, then the geom offset will just be the difference between the home value, and the real diameter of the tool tip. Example: At home the display reads X16.0000, but the turning tool tip is really at a 15" diameter, then it is starting too small, or too negative, by 1.000. So, the geom offset for that tool would need to be X1.000 (a positive value). This will offset or shift the tool path 1.000 larger diameter so that it matches the 16.0000 that the control thinks the tip is starting at.

My control is set up to throw a non-zero number, i.e. 11.9180 into the X position after manual home. So, I gather when I use the MEASUR function on the MDI the control is figuring this difference and plugging that value into the G offset page for me? Therefore, when i use this function the control references home position (or Machine Coordinate System in Fanuc parlance).

As far as Z axis, you can choose where you want the 0 position, or datum, to be. It could be the spindle nose, the chuck face, the jaw face, or the face of the part. For those machines equipped with a tool presetter, it would be the face of the front button. What is critical is that whatever feature is used for the program as Z0, the tool offsets have to be set off that same surface. I would argue strongly for using the finished face of the part as 0. Doing it this way is logical, and makes it far easier to follow the program on the screen. This way, the ABSOLUTE position (the tool's position commanded by the program, including offsets) will read 0 when the tool tip is touching the finished face. If the absolute display is positive, the tip is clear of the part. If negative, it is past the face of the part. If done this way, the GEOMETRY OFFSET for Z represents how far the tool tip must travel from home to touch the face of the part. It would be a negative value, as the axis has to move in the negative direction from home to the part.

If the chuck face were used as 0, then the Z geometry offsets would represent the distance from home to the chuck face. Of course, machining in that area is detrimental to tool life, or machine life, for that matter. So, you would have to have an amount in the WORK/EXTERNAL/SHIFT offset to back the tool path away from the chuck. The amount would be the distance from the chuck face to the part face. I don't like this method, simply because if that WORK or SHIFT offset is destroyed (set back to 0), the tools will be diving into the jaws. However, the method is valid, I just think it's less tolerant of human error. Because I earn most of my living fixing machines, I tend to have great consideration for things that can go wrong and tear up machines, otherwise called failure modes. Wrecks are almost exclusively caused by human, not machine, failure modes.

Yep, all the wrecks I've had were caused by me.

 

[WayneC369]

Okay, so now another question comes to mind: Why would there be a -3.0000" for Z at it's home position? There's only roughly .200" more travel to go before the limit is hit. Why not Z0.0000" instead????

 

[Ox]

I kant help you with the "measure" thing as I have never used it, but if you want to change the HOME position, you can easily find that parameter and change it. Looks like 1240 - 1251 to me.

I have changed them on a cpl other machines before.


On your "Settings" page - top line - set PWE to write.
Hit the SYSTEM key and scroll down to your param #


Keep in mind that if you move the value much - you may need to change the limits on your Software O/T params as well. Editing out .089 may not be much of an issue, but if you get a burr and want to change your Z three inches - that could be an issue.



---------------------

Think Snow Eh!
Ox

 

[WayneC369]

I kant help you with the "measure" thing as I have never used it, but if you want to change the HOME position, you can easily find that parameter and change it. Looks like 1240 - 1251 to me.

I have changed them on a cpl other machines before.


On your "Settings" page - top line - set PWE to write.
Hit the SYSTEM key and scroll down to your param #


Keep in mind that if you move the value much - you may need to change the limits on your Software O/T params as well. Editing out .089 may not be much of an issue, but if you get a burr and want to change your Z three inches - that could be an issue.

I'm not sure what exactly the MEASUR function is doing, Ox. But, it does seem as though it references the center line of the spindle when setting tool offsets in the X direction. I can't make any sense of what I see while setting tool length offsets. I don't think I will change any of the parameters in that area until I gain a much better understanding of what's going on.

As a side note I found that if you press the "Spindle Stop" key it will shut that annoying beeper up while PWE = 1. I saw the CRT had been replaced with an LCD display and noticed color during boot up and monochrome during operation so I flipped the bit changing it to color. That made the whole machine look better!

EDIT - After doing some checking the best I can tell the MEASUR(e) function references the spindle axis for X offsets and machine home (or machine coordinate system in Fanuc parlance) for Z offsets. After taking a facing cut and using the MEASUR(e) function to enter the offset I sent the turret home. The relative counter zeroed out. Then handwheeled the turret back to the part face. W then matched the Z offset for that tool.

 

[alphonso]

The 18 series MEASUR is an updated and easier to use sequence from 0T controls: MX(Z)___, MEASUR OFSET, input.

 

[Ox]

So what does that doo?
Just place the U or W values into the offset field that is highlighted for you?
Same as keying it in like I said - or something different?


-----------------

Think Snow Eh!
Ox

 

[Greg White]

I have had my Yasnac(Fanuc based?) for 0ver 3 years or so,never used that "measure gizmo'
Messed with it once tool started heading for table,havent tried again,
so much to learn,so little time...
Gw

 

[WayneC369]

So what does that doo?
Just place the U or W values into the offset field that is highlighted for you?
Same as keying it in like I said - or something different?

Ox,

I'm so confused about this right now that I'm not sure if I should be scratching my ass or winding my watch!

I hope you don't think I'm dismissing your method here, I'm just thinking out loud. Besides, I have yet to make any chips as I'm still learning. I eluded to this earlier, but here's the steps as I've figured them out using the manual (which is a NIGHTMARE ):

For setting part Z zero flush with back/chuck end of part:

(1) Pick a tool and take a facing cut. (in my case it's T1 with a trigon insert)
(2) Don't move the tool in Z but get it clear of the part in X.
(3) Measure the length of the part.
(4) Highlight the Z entry in the Geometry Offset page at the tool position you're setting.
(5) Enter the measured length in this form:"Znn.nnnn" (let's just use 1.0000" for talking purposes, therefore you type in Z1.)
(6) Press the MEASURe soft key.
(7) The control then subtracts the number you entered from the Z home position and puts that number into the Z entry of the geometry offset page for you. Using this method references all Z offsets to machine home position.
(8) Touch off all subsequent tools to the same surface and repeat the entry process for the selected tool.


For setting the X offsets:

(1) With T1 turn the OD of a part.
(2) Clear the tool from the part along Z without moving X.
(3) Measure the OD.
(4) Highlight the X entry in the Geometry Offset page at the tool position you're setting.
(5) Enter the measured diameter in this form:"Xnn.nnnn" (let's just use 2.0000" for talking purposes, therefore you type in X2.)
(6) Press the MEASURe soft key.
(7) The control then calculates the difference between the spindle centerline and the actual turret position and enters this into the geometry offset page at the tool position you have highlighted.
(8) Touch off all subsequent tools to the same surface and repeat the entry process for the selected tool.

That's what I think I know...

Now, I'm still trying to digest the Work Offset and how it works. I think I've got the steps down, but without understanding how it works. After manually homing the turret I saw my Z change from -3. to a + number that was the same as the Z offset for T1 only it was positive instead of negative. After entering a few codes to test turret movement I homed the turret and now Z reads 0!!! I used your header and I'm thinking that's what zeroed Z when at home position.