DeaWoo Lynx 210A Setup

Hi guys,
So, I bought a DeaWoo Lynx (Because I have 2 Machining centers from them and love them), and the saying is true I think. "You can turn a lathe guy into a mill guys but not a mill guy into a lathe guy"..haha.
Anyway, I have run a few jobs on this machine but I dont set it up very often. Once every 4-6 months. So, I forget the tricks.... etc. And, I dont think I ever really set it up correctly. For instance, the Tool setter arm. I didnt use that ;) I'm not even sure how I got it to run correctly but I know I made alot of adjustments to do so. So my question for you guys is, can you tell me how to set it up? I have looked for videos on youtube and searched and even got the setup procedure from my DeaWoo Dealer but still just dont seem to get it.

I know there is a very specific procedure you must follow in order for the setup to work.
First off, the reference point. Is this just a reference point out in the middle of no where?
How do I locate my fixture offset?
And from there, I believe, I should set the first tool off the part (finished cut) and somehow teach the machine...? Then each tool off the pre setter and it will calculate all the offsets....? Idk. But I was pulling my hair out this morning ;)
Anyways, thanks for your help guys.
Tom

The reference point is a known location where the face of the turret is a specific distance from the face of the spindle, and the ID holders should be on center when X is at 0. There should be a diagram in your manual. If you can't find one, get me the serial number, and I'll send you one.

Set all the tools off the Q-setter. Then, activate any of the qualified tools (I usually use the finish turning tool, say tool #1) by MDI - T0101EOB Insert Cycle Start. Now handwheel Z over to touch the face of the part. Go into the Work offset display, move the cursor to G54, and type Z0 then [MEASURE] softkey. Your Z absolute should now read 0. If so, then all your tools now know where Z0 is. Now make parts.

Thanks for your reply.

Ok, I will look into the reference point because I think this is the root of my problem.

I was able to set up my first tool and I think I understand how to go through the rest of the tool "but" in the set-up procedure given to me from my Doosan dealer, it tells me to jog the tools .1-.200 from the Q-setter and then use the jog key to jog it in. But when I try, the machine does not move. Any idea why it will not move? I put it in "jog" mode and nothing... I was under the impression the machine would recognize when the tool tip was touching and stop the jogging process. But it will not jog at all.

Thanks,

Quote:

---

Originally Posted by dcoupar

The reference point is a known location where the face of the turret is a specific distance from the face of the spindle, and the ID holders should be on center when X is at 0. There should be a diagram in your manual. If you can't find one, get me the serial number, and I'll send you one.

Set all the tools off the Q-setter. Then, activate any of the qualified tools (I usually use the finish turning tool, say tool #1) by MDI - T0101EOB Insert Cycle Start. Now handwheel Z over to touch the face of the part. Go into the Work offset display, move the cursor to G54, and type Z0 then [MEASURE] softkey. Your Z absolute should now read 0. If so, then all your tools now know where Z0 is. Now make parts.

---

What is the control make/model # and machine serial #?

DeaWoo Lynx Lathe setup with Q-setter

Tool Offsets
1. Zero out fixture offsets.

You must touch off on all tools prior to touching off on the stock

2. With the turret in the "home position" (or reference return position) from MDI, select first tool to be measured.
T0101 (in my case).

3. Bring Q-setter down. And navigate to the "Tool Offsets" Page

4. Touch tool off. The tool and axis you touched off should be highlighted in the "offsets page".

5. Press and hold "Tool Measure" hard key on Operator panel.

6. Now, type in X0 or Z0 and hit the Measure soft key. Your offset should automatically be calculated and inserted on the proper axis which your "Handel or Pulse generator" was jogged to. If you did not zero out your fixture offsets, the machine will have compensated for them. And your offset will be wrong.

7. Now jog the turret to a safe location.

8. Select MDI on your operator panel and call up your next tool. T0303;, T0606;, T1010;

9. Repeat steps 3-6.

Work Offset
1. With the turret at a safe location, In the MDI page, call up a tool your going to use for facing and the Fixture offset, G54 T0101;

2. Turn spindle on, M3 S1200;

3. Jog facing tool to part and take a light cut.

4. Highlight specific axis

5. Press and hold "Tool Measure" hard key on Operator panel.

6. Now, type in X0 or Z0 and hit the Measure soft key. Your offset should automatically be calculated and inserted on the proper axis which your "Handel or Pulse generator" was jogged to.

7. On the X offset, you want to add in the Dia of the stock. This way the offset will be right to the center of the stock. You can do this by typing .xxx and then pushing the softkey "+input".

Its a Fanuc 18i
The serial # is LC2103084 (I think. Doing that from memory)

I got the etire setup down now.

But the one thing I dont understand is why the drill X offset would change from "zero" to well, "zero" and be a mile off after I figure out the fixture offset...? Before the fixture offset was put in place, the "zero" was perfect...??? Scratching my head on this one.

When using the Qsetter I dont think you need to use the Tool Measure hard key or type in X0 or Y0 you just touch your tool off the probe tell it beeps or the light comes on it it should put the correct offset in for you at that point. I think the hard key and the measure soft key only need be used when you are not using the Qsetter. This may be why your X0 for your drill is off

on your G54 dont use the X when you measured your tools on the Qsetter that took care of your X offset all you need to do is Z

I have attched a file I made for my operators to us when setting up the machines that should help you

well it appears that that file is to big if you will give me your email I will send it to you

Thanks Chucker.
Your probably right about the hard key. I will test this out on my next setup. However, the manual tells me to jog the tool to .1-.2 from the Q-Setter and then use the jog key (not handel) into the Q-Setter. BUt my machine does not move when I try to use the jog keys. Idk. So, I just skip that and move it in with the handle. It also does not beep. I'm not sure if my machine set up to use the jog keys and have the Q-setter beep. Its a 2004 year machine so......

"on your G54 dont use the X when you measured your tools on the Qsetter that took care of your X offset all you need to do is Z"
I dont follow you on this.... Do you mean, dont Touch off on the dia of the part and register an offset in the G54 X position? How would the machine know where the stock is? I understand how it knows where a drill is (becuase the boring tools are all X axis cetered). But for a cutting tool it would be way off....

Here is my e-mail,
Tom@QTS Frame.com

Thanks!!

Quote:

---

Originally Posted by chucker

When using the Qsetter I dont think you need to use the Tool Measure hard key or type in X0 or Y0 you just touch your tool off the probe tell it beeps or the light comes on it it should put the correct offset in for you at that point. I think the hard key and the measure soft key only need be used when you are not using the Qsetter. This may be why your X0 for your drill is off

on your G54 dont use the X when you measured your tools on the Qsetter that took care of your X offset all you need to do is Z

I have attched a file I made for my operators to us when setting up the machines that should help you

well it appears that that file is to big if you will give me your email I will send it to you

---

When you measure tools from the Qsetter in X you are telling the machine the machine where center of yor part is for that tool thats why you dont need the G54 X when you measure you tools in Z on the Qsetter you are just telling the machine that they where all measured from a kown point just as if you had used the face of the chuck then your G54 Z moves that point to the face of the part.

I will send you that setup file today some time

I would recommend to determine the offset of any tool without a tool setter to understand the concept of the offsets on the lathe. If you do not understand the basic with a single tool then you will always make confusions on the future = some collision. At the end all makes sense, and if you are secure, then move to the tool setter.
In my set up I have a tool that I call master tool and it is used only for facing. This tool have offset z=0 and all the remaining tools are calibrated in relation to this one.