| Forums | Sign Up | Reply | Search | Statistics | Home Page |
Online now: Guests - 2
Members - 0
Most users ever online: 82 [5 Sep 2013 00:45]
Guests - 82 / Members - 0
Integrex General www.integrexmachinist.com community built on miniBB / Integrex General /

How do you touch off a roller box turning tool?

 
Stuart
Forums Member
#1 | Posted: 11 Oct 2009 00:09
Reply 
I need to machine some 0.24" diameter parts 4.5" long and I was planning to try a recently acquired roller-box turning tool. As it turns out, I guess I've never had to physically touch off a tool by the cut and try method since all my CNC lathes have had tool presetters. I can establish the length for the Z axis dimension easy enough by touching off the face of the roller supports. I can't for the life of me figure out how to set the diameter of an OD turning tool so it uses the machine centerline for X0.

On my Hass, I just hit F2 and it inputs a predefined value. How do you do it in Mazatrol? Where do you come up with the value.

I plan to turn a pointy end on a shaft, transitioning to the .24" dimension for .3" or so. I figured I would set up the tool on centerline, and jog over the machined area, then adjust the roller supports so they just touch, and finally adjust the insert so it cuts to .24" diameter.

In use I'll bar pull the stock out the required amount. Feed onto the stock with the box turning tool, and feed off at 3X the infeed.

Any ideas on how to set up the tool, or actually use it. I've got a couple thousand parts to make and it's not worth finding someone with a screw machine at this point.

Thanks,

Stu
jimiscnc
Forums Member
#2 | Posted: 11 Oct 2009 05:56
Reply 
You need to have two dimensions on your box tool. The distance between the touch off point in both X and Z on what can reach the tool eye. Then you need the distance from this to the desired set point on your cutting tool.

After touching off the edges you can get to, go in and incrementally adjust the set values of the taught X and Z offset. In X, all offsets are diameter values, so the number has to be doubled. Z is always the actual true distance. These adjustments are the dimensions for set point to desired set point on the cutting tool.

Write numbers down and think through whether plus or minus numbers should be taught.

An example:

A neutral turning tool. 60 degree insert. 60 degree leading and trailing angle. The set point in Z cannot be touched off, but the side of the tool can. For a 1" square shank tool, touch off the side of the shank in Z. That sets the edge of the tool as the driving point in Z. This value is off by .50000". arrow to the Z offset register, turn on the incremental switch, and input -.50000". This incremental adjustment has now brought the Z offset value to match the Z cutting point, which is the center of the tool.

An example in X.

A .50000" dia gage pin in a drill collet holder, oriented in drilling at main spindle. Touch off X at the 12:00 position on the tool eye. This sets the lower circumphrence as the set point, but you want to set the centerline as the set point, for a drill. Arrow to the X register, incremental s/k switch on, key in -.50000" -input. Now the X offset is driving the centerline of the holder/gage pin.

If you touched off the 6:00 tool eye position, then you would incrementally adjust by .50000", a positive number in this case.

12:00 tool eye is also known as X minus. 6:00 tool eye is X plus. 3:00 is Z minus, and 9:00 is Z plus. So named because thats the direction the axis must take to make a reading.

Write the numbers down and do an eyeball MDI position check to make sure you got the +/- and value correct. Remember - all X is diameter numbers, not radial (aka true distance)

-90% Jimmy
Stuart
Forums Member
#3 | Posted: 11 Oct 2009 14:46
Reply 
That makes sense, but let's say I'm using a simple collet holder. If I call the tool a drill, center drill, or an end mill, I only need to touch off the tip of the tool. Mazatrol doesn't even allow you to touch off a diameter and places a symbol for the value.

In a Mazatrol program when you tell it to go to X0 for example, the control places the tool tip on the machine centerline. It's automatically using some value that is stored somewhere. That's the value I want to input for the box tool. If the box tool isn't on the exact machine centerline, I can't see any way it will work properly.

I'll probably just lie again and call the tool a turn drill, and write a manual process. Turn Drills only needs to know the length and it should be on the centerline. It would be nice to not have to lie and cheat to run a simple machine though...

I suspect there is a way to take an outside cut with a turning tool, and without shifting the X point store that value somehow and then measure the machined diameter with a micrometer and comp the originally stored value. One of you gurus care to enlighten me please, pretty please....

Like I've said, I've always used a presetter. Just another hazard of the self taught route.

Thanks,

Stu
jimiscnc
Forums Member
#4 | Posted: 11 Oct 2009 16:29 | Edited by: jimiscnc
Reply 
I remember more about Integrexes now. The above method applies mostly for fixed tool turret type lathes. Like, I'm pretty sure it applies to the lower turret on Integrexes, which is usualy just a two axis lathe type turret.

Your machine is probably tool length expressed as Length A and Length B. These values are from the datum face and centerline of the turret face centerline and are the dimensions that would be used from an offline tool presetter. A is axial and B is radial, to the turret axis.

there is a way to convert the Tool data from one system to the other. I suspect it is in the set-up tab in the windows pull down on the Tool Data page? If not that, then a parameter or something else obscure.

It's a moot point. plan B for you would be to turn down a diameter the box tool could fit and also face off to Z zero. Bring the tool point to cut on the known diameter (it's gotta be measured after you turn it) so that it's barely making a mark in the bluing you put on. Go to tool data and cursor over to the length B column and turn on the teach softkey switch (turns magenta) key in (Measured diameter number) and it should calculate the correct length B number. Touch the tool point off the Z zero face and teach 0 when the tool point is dead nuts on Z zero and that should give you the correct Tool Length A.

Also, the tool should be named 'other" or "special", so Mazatrol doesn't make some assumptions like you describe with your fixed drill.

To summarize - the teach function in tool data should give you the correct length A and B numbers if you bring the tool point in X and then Z to a precise known position off your part. The check if you got it right is, after teaching each axis, but before moving, the position display should show the correct X and then Z numbers based on the part you used to touch off.

-90% Jimmy, again.

You said

"I suspect there is a way to take an outside cut with a turning tool, and without shifting the X point store that value somehow and then measure the machined diameter with a micrometer and comp the originally stored value. One of you gurus care to enlighten me please, pretty please...."

i tried to describe this method above. The trick is that you can only get to the TEACH softkey when the cursor is in the Length A or B window you are setting.
Stuart
Forums Member
#5 | Posted: 11 Oct 2009 17:52
Reply 
I knew there had to be a trick! That helped a bunch. Many Thanks!!!!!!!

Having never used a box tool before, it's a wickedly cool tool for this application. I can tell I'm going to need to grab another half dozen or so and just leave them set to the standard diameters I need to turn to. Stinking fast, and no defelection, so the parts are pretty darned accurate.

Now to make a parts ejector that doesn't bounce the tiny parts off the front wall of the machine...

Stu
jimiscnc
Forums Member
#6 | Posted: 12 Oct 2009 09:33
Reply 
I'm an ex-Mazak guy and I used to be paid to be a freeking guru. One of the greatest sources of satisfaction was being able to solve control related issues. In my 6.96 years there I only had one mazatrol problem I could not solve! (actually, it was not always my own work - many times I turned to my knowledgable colleagues and got them to solve the prob)

I eventually learned that all Mazatrol things have solutions, if you were willing to dig deep enough to find them. Mazak has tremendous internal corporate info resources and it was wonderful to have access to them!

Thanks for the feedback on your success. The integrex is a magnificent beast, and that Length A and B business was evolved from the M-Pro control, which was on really big machines I didn't work on much. M-Pro was evolved from a machining center to a lathe, as opposed to the MT-Pro, which was evolved from a lathe into a m/c. Mazak tried to consolidate the separate control evolution trees with the Matrix.

-90% jimmy

And now I'm slowly restoring a used VQC-15/40 with M-2 control, so I can continue to put food on my family.
Stuart
Forums Member
#7 | Posted: 12 Oct 2009 12:21
Reply 
I've always been amazed at how bright certain Mazak personel are. Unfortuantely, you need to wade through far more of the "not so bright" types to find the gems, and of course you need to know whether what they are telling you is BS or not. Life would be so much simpler if people just say "I really don't have a clue, but let me put you in touch with the person who does, and then they actually get you to that person.

In the Integrex world, it seems we call LA, they call Kentucky, who calls Mazak Japan, who calls the individual vendor who sold, designed and installed the component, who calls back to Mazak Japan, who calls Kentucky, who calls LA, who calls me back... if somewhere along the chain of events, the message didn't get lost or misplaced....

Thanks for your help, the part worked great and I'm reworking the program into half a dozen more lot sizes. I'm not going to get rich with it, but it will provide yet another repetitive job to fill out the spindle time when it would otherwise sit idle anyway. It also saves me from having to go seek out a screw machine for a while longer.
 

:);):-p:-(More smilies...  Disable smilies in post
Your reply
Bold Style  Italic Style  Image Link  URL Link 

» Username  » Password 
Only registered users are allowed to post here. Please enter your login/password details upon posting a message, or sign up first.
 

Forums are powered by miniBB®