[Desertrunner]

fordav11

I think your initial 'trouble' with tool setting using the probe is that the probe is not calibrated so using it gives incorrect values. use the manual tool setting method I described above. once you have that working the procedure to calibrate the probe can be followed and you can cross-reference your correctly set tools to make sure the values are the same.

That makes a lot of sense, the guy will bw here in 4 days and I will come back to you on what he says is the problem.
Thanks for the help its much appricated.
Tony

[Desertrunner]

Hi Guys,
Set all the tools okay but I find the turning tool and the drills are 1.7mm out. In other words if I set "Tool 1" (its a outside turning tool) to be correct then all the tools that rely on centre line are out. If I set based on a drill then the actual cut part using the turning tool will be 1.7mm wider. Have a Udrill and it cuts perfect its in "Tool 7" then when I cut the outside of the part aiming for a final Dia of 30mm I get 31.7mm using Tool 1.

It is possiable that its the tool setting arm, how do I check it?
Tony

[fordav11]

if you use the manual tool setting method is it wrong? I suspect not.

if you are probing then yes your setting arm is not calibrated.
if X is out by 1.7mm then it means your parameter for X+ is out by 1.7mm.
That's parameter 5015.
check and list your parameters 5015, 5016, 5017, 5018

you can probably fix it easily by subtracting or adding 1.7mm to either 5015 or 5016

the numbers have no decimals so 789123 = 789.123mm

if in doubt take a photo of the parameter page showing 5015-5018

also each tool has it's own individual X setting so if one tool is set wrong the others should still be ok. as I said the center line does not move. the tool reference position moves and each tool X reference (i.e. X geometry offset) is separate from the others.

another quick fix is to put -1.7mm on your G54 X
technically G54 X should be 0 but you can offset all of the tools using the workshift if you want to.

you can check the setting arm by moving the tool to the setting probe and note the X position on the readout. Then set the X geometry for that same tool manually and note the X geometry offset. The 2 numbers should match. If not your probe is out by the difference between the 2 numbers. Add or subtract that number from whatever number is in parameter 5015 and that'll fix your problem.

[fordav11]

you can put an offset on Y for that tool or if all tools are the same put something on the G54 Y

[Desertrunner]

I am not sure if its called "3" instead of Y, it seems the angle of the boring bar tip is not contacting the surface at the correct angle and it shuddering. I will have a look at G54, thanks. In the manual for the lathe it talks about the "Keep Relay" to K13.0=1. In the next sentence it said "Press Spindle override VALID/INVALID button several times to unclamp the turret." By the way I forgot to mention when I got the lathe tool 2 shows up as tool 1 on the controler.

Tony

[fordav11]

are you sure you have Y? If this is the same machine that you show screens for above then you don't have a Y axis.
3 is the turret servo
If the tools don't line up to center then you need to get your maintenance people onto it, pull it apart and re-align the turret properly.

[Desertrunner]

Ford,
Yes its the turret servo and its "3", I have been playing around with "Grid Shift" in the parmeters. I am waiting for a dail guage to arrive but it seems that I can raise or lower the turret centre line but using this parmeter. I played with it on the weekend and it seem to move it I just need a dial guage to double check it. Its pretty funny I have this machine as a hobby/work machine so its just a interest, today I went to a machine shop that has a CNC machine they use every day. Turns out they don't have a clue how to adjust there machine so will be helping them realign these as well.
Really appricate the help you gave me pointing me to the parmeters to adjust the tool setter it was a great leap forward for me.
Tony

[fordav11]

grid shift doesn't move the turret. it can move the servo but thats the wrong way to fix your problem. there's a mechanical lock holding both turret and turret body together. search google for 'curvic coupling' and you will see what it looks like. its basically 2 castle nuts that mesh together and the 'castle' ring that sits inside the turret is located with tapered dowel pins and bolts. do a search on these forums for 'curvic coupling' for some info on re-aligning it.

[g-codeguy]

SQT, never use the same work coordinates for both spindles. You can use whatever work coordinate you want to, but I would be consistent so as to limit confusion with the operators...or yourself. Many use a 2nd tool with Z0 Geom., but if you have a good touch probe, then use it. The tool does not need to be set at Z0 in order to set work coordinates for either spindle. I do not call them work coordinates, but workshifts....probably not the correct word to use, but I learned on single spindle lathes and workshift is what we called it, not work coordinate. Anyway...when setting the workshift, instead of typing in Z0, you type in the actual value of that tool's Z-Geom.

EDIT: I agree. The Fanuc manual can be a pain to understand at times.

[fordav11]

on some machines you can actually set the workshift with any tool as long as it is already set. it works on my machine (Mori) but on others it would be necessary to either have one setting tool with a Z0 geometry or set the Z0 workshift to the number in the Z geometry for that tool. With the latter it can get confusing if the place where you touch the tool is not Z0 then you have to add or subtract a distance from the Z geometry of that tool in order to achieve the correct workshift calculation. It's a lot easier to just have one tool with a zero Z geometry :-)

[g-codeguy]

on some machines you can actually set the workshift with any tool as long as it is already set. it works on my machine (Mori) but on others it would be necessary to either have one setting tool with a Z0 geometry or set the Z0 workshift to the number in the Z geometry for that tool. With the latter it can get confusing if the place where you touch the tool is not Z0 then you have to add or subtract a distance from the Z geometry of that tool in order to achieve the correct workshift calculation. It's a lot easier to just have one tool with a zero Z geometry :-)

SQT, let's use a Hardinge with an OT control as an example. Say you have probed the tools and want to touch off with the 80 degree roughing tool. Its Z-Geometry is .2516. Touch off the tool. On the workshift page, type in MZ.2516, press INPUT hard key. Your workshift is now set correctly for all tools. Alternately you could type in MZ0, press INPUT hard key. Then type in W.2516 press INPUT hard key. Your workshift is now set for all tools.

Oops, SQT, your control does not work this way. You should have 2 columns for X & Z on the workshift page. Highlight Z in the right column. Type in .2516, press INPUT soft key. Workshift should be set for all tools. Alternately type in 0, press INPUT soft key (while right column Z is highlighted.) Cursor to the left column Z. Type in .2516, press +INPUT soft key. Workshift is now set for all tools.

Setting the workshift in G54-G59 is done similarly. On our Daewoo you would highlight Z in G54. Type in Z.2516, press Zero hard key, press Zero soft key. Workshift is now set for all tools. Alternately type in Z0, press Zero hard key, press Zero soft key, type in .2516, press +INPUT soft key. Workshift is now set for all tools. Not all lathes have the Zero hard key. Some controls have a Zero hard key and use "Measure" instead of "Zero". I hope I remember correctly. Can double check Monday. Or someone will correct me if I am wrong.

Our 16-TT controls do not have a Zero hard key. Neither does our 21-T control lathe. Workshifts are set using the method described in my 2nd paragraph.

[fordav11]

you quoted me before your explanation but A. I already know all of that and B. I'm not SQT. he has not been seen here for a week.....
and yes you can use input+ to correct a workshift. touch the face of the part and set Z0 then use input+ to add or subtract an amount. I do that on our Fanuc 0's that only have the simpler workshift screen without G54-G59

[g-codeguy]

you quoted me before your explanation but A. I already know all of that and B. I'm not SQT. he has not been seen here for a week.....
and yes you can use input+ to correct a workshift. touch the face of the part and set Z0 then use input+ to add or subtract an amount. I do that on our Fanuc 0's that only have the simpler workshift screen without G54-G59

I realize that. My fault for not explaining why I quoted you. I was trying to expand on your explanation for SQT's benefit. I've read your posts before and already know you have more knowledge than I will ever have. Especially considering I don't have much longer to work before retiring. :wee:

I've only worked at one shop...28 years now. My experience is very limited compared to most on here. I try to help when I can, which isn't often.

[gbowne1]

I've been dealing with this on the 10TF lately... how?

[fordav11]

dealing with what specifically?

[gbowne1]

I've been dealing w lately tryin to learn all the wear, geometry, tool, work, etc. offsets on the 10TF.. so, just so you know, I'm used to a older version of a 0T-C and the large lathe had a 16TTF.. where I did some training at for 3 months.

I think I'm following this thread ok. I've been trying out some sample programs that some have forwarded me. As the CNC lathe is kinda new to me.

I'm tryin also to figure how its set up w/ U, V, W, A, B, C.. on, my machine. I do see the label B on the Axes DROs.

Im working from scanned exerpts from the 10/11/12 lathe manuals.

[fordav11]

UVW is incremental on a lathe. you just put U for incremental X movement and W for incremental Z movement. V relates to the Y axis if the machine has it (normally with live tools as well)
with live tools and rotary chuck C axis you can use H for incremental C movement. A or B on a common lathe doesn't normally exist although it could be used by some specialist machines for another rotary axis. Usually A and B are used on a mill but B is used on a 5 axis lathe/mill as the main tool head rotation axis.

regarding 10T info, the closest manual in pdf is the 15T-B. almost everything is the same so you can just read the 15T-B manual for 99.9% of the required info.

[gbowne1]

I have only a few 15 Model B manuals and they are for the M type only.

I dont know why B is there. I didn't have it set up that way. It's just a standard 2 axes CNC lathe w/ a 8 tool turret and about the size of a 13x40 although the machine itself looks like one of the 80s Mori Seiki SL lathes.

[fordav11]

you can get a full set of 15B pdf manuals here....
www.prodsa.com.ar - /integradores/Manuales Tecnicos/Servo_FANUC_Motion/CNC/CNC/iDocs for CNC/LEGACY CNCs/Series 15 Model B/

[gbowne1]

Thanks fordav.. ill get those. I have just about every other FANUC book available online, but not those.. I'll get back with you on the FAPT too.

I also recently got the manuals for the machines' turret. Fixed a couple issues, especially chuck open/close..

So setting x to diameter and z to the offset will work. As long as the G54 is set right will work with the measure.