Nakamura Fanuc 6T has a few questions

Back again. Ok so my Kitamura OMB is still down, waiting on Servo RAM Chips, my Nakamura TMC-15 is down with a blown spindle drive, so Im messing with my other machine (thank god my Lancer is still up and running). I have a 1985 Nakamura Slant 1 with a 6T control. Its the older, bigger brother that came with the TMC-15.

I have never ever messed with a 6T control. Its always been O series or newer. I put a few tools in, got the offsets correct (Should also mention that X axis is backwards, but thats in another thread, seems that Naka made a lot like this).

Tool changes have me a little perplexed, and I think I have it figured, but wanted to make sure. If I command a G28 U0 W0 the machine will home, If I call tool T0202, the turret indexes to T2, then moves down the amount of the offset, essentially taking the tool tip to X0Y0.

I went through a bunch of programs that were in memory on the machine, and it looks like G50 has to come into play. Assuming that there is no "work offset" then I have to call the coordinate system with every tool change? Im assuming that a tool change needs to look like this:


G28 U0. W0.
T0202 G50 X(tool offset amount) Z(tool offset amount)

Ive tried this in MDI and it looks like it works and the turret indexes then stays put, which is what I want, no crashes. Just wanted to verify Im not doing something silly. Ive done some manual turning on here with the handwheel and the machine runs great, but its time to get some DNC hooked up and make some of my loan money back!!

Thanks

Attachment 380700

anybody?

Hi Third-Gen,

Can you list a G-code program with a few tools, that makes it a little easier.

Regards,
Heavy_Metal.

I dont have any code made for this machine, the only code I have any example of is what was stored in the old program memory for the machine. Next time im over there ill remember to copy some down. its just odd to me that there is a G50 at every tool change. But it kinda makes sense that there is no work offset at all (like on my 0T lathe) and you essentially have to "grid shift" the entire coordinate system to correspond with each tool once its called. Gonna make setting up lots of one off parts a complete pain in the ass.

Quote:

---

Originally Posted by Third-Gen

I dont have any code made for this machine, the only code I have any example of is what was stored in the old program memory for the machine. Next time im over there ill remember to copy some down. its just odd to me that there is a G50 at every tool change. But it kinda makes sense that there is no work offset at all (like on my 0T lathe) and you essentially have to "grid shift" the entire coordinate system to correspond with each tool once its called. Gonna make setting up lots of one off parts a complete pain in the ass.

---

Hello Third-Gen,
The only FS6 control that had Geometry Offset Programming was the 6M (Machining Centre) Model B control. When it still exists on the control panel, Model B (T and M Series) control is identified with a Yellow Fanuc System tag. When this is missing, the sure fire method to identify the control as a Model B is that a whole page of program code is displayed when in Auto Mode (similar to what you see in Edit Mode); only the current and pending Block is displayed in Auto Mode of a Model A. From the picture of the machine in your first Post, the control appears to be a Model B.

Irrespective of the Model (A or B), of your Series 6T control, it uses G50 to set the Coordinate System for the machine. This setting system was originally designed to use the Tool Offsets for wear only and in fact, many machines are set so that there is a limit (small) to the value of the Offset that can be registered. In most (if not all) 6T controls I've seen, calling a tool with the Offset included in the call command, T0101 for example, will move the X and Z axis the amount of the Offset during the Tool Index. Accordingly, its better practice to Call the Tool without the Tool Offset and apply the Offset in the first Motion Command. In this way the Offset is applied seamlessly. Following is a fairly accepted method of setting the Coordinate System and applying the Tool Offset.
(FIRST TOOL)
N1 G18 G21 G40 G99
G28 U0.0 W0.0
G50 X300.000 Z400.000
G50 G00 T0100 S2500
G96 S250 M03
G00 X150.000 Z10.000 T0101 M08
G01 Z1.000 F1.0
-------------------
-------------------
-------------------
G00 X300.000 Z400.000 T0100 M09
M05
M01
(NEXT TOOL)
N2 G28 U0.0 W0.0
G50 X250.000 Z350.000
G50 G00 T0200 S2500
G96 S250 M03
G00 X50.000 Z10.000 T0202 M08
G01 Z1.000 F1.0
-------------------
-------------------
-------------------
G00 X300.000 Z400.000 T0100 M09
M05
M01
and so on.

I like to make each Tool Operation a Stand Alone program, as it aids greatly when having to repeat a Tool Operation (adjusting an Offset and re-cutting the feature for example). Its important that the Tool Offset be cancelled when the Tool is returned to its Start Position (where the G50 was used to set the Coordinate System). Failure to do so will result in a gradual (the size of the Tool Offset) shift of the Workpiece X/Z Zero.

Regards,

Bill

Bill, your example appears to be what was in the machine from some of the older programs in memory. I guess ill have to put a whiteboard by the machine to write all my offsets down since I do mostly hand programming. Glad the 0T machines have geometry offsets, makes life so much easier. I looked and looked and couldnt find any way to do an actual geometry offset, but I can set the ORIGIN to where i need it on the POS pages, but im not sure if using that along with G50 is gonna muck something up. Ill have to give it a try and keep the feedrates and rapids turned way down.

And yes, if I call a tool, T0101 and have the offsets set like a standard lathe with large values, the tool will immediately move to the programmed zero point from where the offsets were measured. thats when the G50 started to make a little more sense. ill have to remember to call the tool with no offsets, or just leave them all 0s and keep them on a whiteboard.

[QUOTE=Third-Gen;2124004]Back again. Ok so my Kitamura OMB is still down, waiting on Servo RAM Chips, my Nakamura TMC-15 is down with a blown spindle drive, so Im messing with my other machine (thank god my Lancer is still up and running). I have a 1985 Nakamura Slant 1 with a 6T control. Its the older, bigger brother that came with the TMC-15.

I have never ever messed with a 6T control. Its always been O series or newer. I put a few tools in, got the offsets correct (Should also mention that X axis is backwards, but thats in another thread, seems that Naka made a lot like this).

Tool changes have me a little perplexed, and I think I have it figured, but wanted to make sure. If I command a G28 U0 W0 the machine will home, If I call tool T0202, the turret indexes to T2, then moves down the amount of the offset, essentially taking the tool tip to X0Y0.

I went through a bunch of programs that were in memory on the machine, and it looks like G50 has to come into play. Assuming that there is no "work offset" then I have to call the coordinate system with every tool change? Im assuming that a tool change needs to look like this:


G28 U0. W0.
T0202 G50 X(tool offset amount) Z(tool offset amount)

Ive tried this in MDI and it looks like it works and the turret indexes then stays put, which is what I want, no crashes. Just wanted to verify Im not doing something silly. Ive done some manual turning on here with the handwheel and the machine runs great, but its time to get some DNC hooked up and make some of my loan money back!!

Thanks

Attachment 380700[/QUOTE

G00 G28 U0
G00 G28 W0
G50 S1000 X0.0 Z0.0( Spindle cap cancels absolute figures x.z )
T0200 (Tool no offset)
G00 X100.0 Z10.0 M03 S100 G97 T0202(pick up offset from Geo screen )
()

(Try and stay away from putting x and z values in g50 for tool geo )

ahh makes sense with calling the tool with no offset, then adding the offset on the first move. ill have to try that.

on that note, whats the main difference between using a g50 and setting X and Z origin with the "origin" function?

did a little more messing around with the machine a few nights ago. heres what i figured out so far.

I measured all my tools off the face of the turret using a Z setter and the spindle nose. all Z offsets are positive value (away from turret)
i turned a diameter, measured, then added that value to the distance from home and used that as my X offset value (also positive since Nakamura is backwards, ill fix this eventually)
calling a tool with T0200 calls the tool but doesnt move the X or Z (which is what I want)
adding the T0202 with the first X or Z move moves the tool to the correct location (yay)
ive been using G50 to set my work origin. Mainly areas in open space right now for testing, but it looks repeatable, and works with all tools so I think im doing it right. Im just not sure if I need to do it with the tool offset applied or not, guess im gonna play with that more later, but it looks like itll do what its supposed to.

the only thing I have to remember with this machine is to home in X before Z. the back side of the turret has all sorts of marks from where it ran into the tailstock, and its moved back as far as it can go. I may try to take the nose off since I dont hardly ever use it.

Thanks shingleton for the advice, looks like thats the way to go. I have no idea what the old programmer was attempting. Ill take some screen shots of the old programs that are in memory and you will all probably scratch your heads.

OFFICIALLY running parts. Thanks for the help guys!! Just need to figure out how to enable the cycle start with the chuck open to use my bar puller.

Ok the Big Nakamura (as i call it) has been working great. only real issue Ive found is there is no Program List. On the OT control I can see a list of the programs in memory, but on the 6T there is nothing, is there a way to see what programs I have besides writing them all down as I load them?

IN edit MODE press CANCEL and then ORIGIN; you should see the program directory.

Well that gets me a little closer i guess. Still gonna have to write down decriptions but now i can see whats in the memory. Thanks memorymanhttps://uploads.tapatalk-cdn.com/201...d71fffd514.jpg

Sent from my LG-H918 using Tapatalk

Notice that the number on the bottom left is the available memory in characters.

Quote:

---

Originally Posted by memoryman

Notice that the number on the bottom left is the available memory in characters.

---

Good to know. Im so used to the O controls the 6 is a little odd to me.

Sent from my LG-H918 using Tapatalk