Thread milling on a nexus 200 MSY Lathe
We have a new nexus 200 MSY with the matrix controller. Has anyone done any thread milling on the od of a part in the lathe. If so how did you do it?
That depends on!
Yeah, I did on my QTN 250 M Matrix. Yes, I don`t have a Y axis!
That depends on what thread you wanna do- internal, or external, but you can do both either!
There are the tools (milling tools) that you can use like the taps, internal or external. And you can program them like the taps, too.
As for the drive power on your V-milling holder, you can use some "stronger", with ratio 2/1
That`s what I did.
So how did you program it? Mazatrol? Manually? or g-codes?
G12.1 in G code
This should allow you to program it.
This is from memory, but here's what you want to program
index to axial driven thread mill tool
lathe spindle stop
mill mode G code G110? G112? I forget
home C axis (G28 C/H0)
position C axis in degrees to where you want to start the cut, or the point in space in which you want to enter the cut.
IMPORTANT CONCEPT. - G12.1 takes advantage of the rotary C axis and X plus minus machine motions to RESULT in straight line motions on the part. I compare the motion to the roller on a race car lifter following the shape of the camshaft lobes. the cam lobes are the workpiece and the roller cylinder is the milling cutter. lifter can only move up and down (X axis) and cam can only rotate C axis.
IMPORTANT CONCEPT #2 - polar G12.1 is EXACTLY like programming a cylindrical part such as a turned blank mounted on a stationary chuck on a vertical machining center. With X0Y0 being the exact center of the part. C0 degrees is the X axis plus vector , C90 is Y plus axis, C180 is X minus axis, C270 is Y minus axis. This CLOCKING is established by where you program C degrees before you use G12.1. So you can mix stuff programmed by mazatrol X-Y or Mazatrol R/angle coordinates and maintain the timing.
IMPORTANT CONCEPT #3 - on your X-Y "overlay" G12.1 is the X axis IN DIAMETER UNITS! Y axis is C axis in RADIUS UNITS! (aka "true distance") In other words, use letter address C instead of Y, and X remains in diameter, where it would be in true distance if you were doing the exact same thing on your VMC.
engage "soft" preload on spindle disk brake (M110, 111 or 112??)
G12.1 pretty sure this has to be all by itself
G01 X___C___ F20.00 - NEVER ever use G00 when in G12.1 mode
NOTE - Mazak's are smart enough to program the feedrate just like a machining center. Sometimes the F word is in DEGREES PER MINUTE, which is confusing. Then just program away like a VMC, following the above rules, until you're done, then withdraw the cutter radially, then program Z plus away from the part.
disengage disk brake
G code to turn back into lathe mode
G00 to turret index clearance position
The EIA programming manual has some decent metric examples to help in this. It is VERY IMPORTANT to follow the nesting sequence of what you turn on and off.
One cool thing on Mazak's is there's a little symbol on the task bar that switched from a turning tool icon to a milling tool icon as you switch from LATHE MODE to MILL MODE and back.
Because of the nature of the beast, the hardest thing for polar interpolation (NOT COORDINATES! - this is R/angle coordinates, not POLAR MOTION(interpolation) of G12.1) to do is go through the part centerline! A simple straight line starting at X2.0 C0 to G01X-2.0C0 will try to make the C axis do an "instant" 180 degree flip at part centerline simultaneously with X real axis motion going from minus direction back to plus direction.
I'm pretty sure if you include the Z you need for your helical type path it will be just like G17 (X-Y) plane in VMC helical - this makes it understood that the contour arcs and lines is in the X-Y(C) plane while Z interpolates linearly in correct proportion to the X-Y circle. If your Z is -.2 and your X-Y command is for a 360 degree arc, for example, it will have interpolated exactly .050 as X-Y has circled 90 degrees, .1 when X-Y has gone 180 degrees, and so on.
Hope this helps. The flow of the sample program in the EIA book for G12.1 is highly recommended.
-90% Jimmy, the Mazak internet fairie
Just curious if there is a way to this inside Mazatrol? i.e. manual programming?
inside mazatrol program
Yes. Especially on the matrix. I think all it is is a MANUAL UNIT. In the body of a mazatrol program, it is fixed format (certain words must go in certain columns) but the matrix let's you use every available valid G code, and I think every M code. (pre-matrix did not allow all available G codes)
Once the heading of the unit is established - tool call, index position and a few other set up things, the subsequent rows allow G code all the way.
3 or more columns for G codes, 3 or more spaces for axis, couple of spaces for I,J,K, I,D,Q stuff, feedrate, S word and then M/B code at the end.
Matrix - you get G codes as listed in the softkeys, but you can write in any G code that's valid. (don't let the s/k's confuse you)
Pre-matrix - G00, 01,02,03, 04, 33, 40,41,42,98,99 is the entire possible G codes (from memory, guys. the point is that it's abbreviated)
General - pre-matrix there were manual units (lathe only) and milling manual units. I think matrix does not make this distinction?
VERY IMPORTANT FINAL POINT
The mazatrol manual unit is almost the only one within Mazatrol that DOES NOT END BY GOING TO TURRET INDEX POSITION! (at the beginning of the unit there is a y/n for going to index pos or not) Therefore your last command in your manual unit is to position to a plus X and Z point that will allow the turret to index 360 degrees without a collision. Nothing more than what every manual G code programmer would have to do anyway.
Thanks Jim! It took a little creativity but we were (are) able to make this work inside Mazatrol with a manual program. So far so good! thanks,
Originally Posted by 90-percent
Just out of curiosity, is there a Mazatrol canned cycle for thread milling on the Integrex with Nexus control?
Originally Posted by 90-percent
Last edited by mcbassin; 07-28-2010 at 06:35 AM.
Reason: im a dumba**
Integrex with Nexus?
The last three generations of mazatrol are plus, fusion, matrix, from oldest to newest. Nexus is a product line of what could be called "commodity" machine tools - machining centers and lathes. Some m/c names are VCN-410 and 510. Lathes are Nexus QT's, from 100 to maybe even 450? The Nexus concept was to design the disparate groups as a whole and take advantage of parts commonality as much as possible with things like ballscrews, ball nuts, thrust bearings, hydraulics and other "same but different" parts common to CNC's.
Nexus is not the control or one type of machine, in other words. Pretty sure Nexus machines were first Fusion control, then evolved to Matrix control in 2006-2007. I think Nexus has recently been replaced by "Smart machines" or something else with an equally cheesy marketing gimmick name?
The Fusion Manual unit abbreviated the G code set, but on the Matrix I'm pretty sure you can use anything that works in G code programs, including Fanuc type multi repetitive cycles G70 through G76. (not sure on that, though, esp with modern "2 line G76" and others that use sequence numbers to define start and finish lines of shape, the mazatrol manual unit does not use N words, but does number each line, doesn't it? Never tried it, or even thought of doing it, for that matter!) Mazatrol absolutely blows the doors off G70-76 in all respects, in my opinion. Only reason to resort to G70-76 is if you're an EIA power user and a mazatrol newbie. (The "go with what you know" principle, and also the name of a Dweezil Zappa album)
Here's some notes from a generic matrix mazatrol turning book
Note 1: Difference between the Manual Program and the EIA/ISO Program
The manual program can be prepared the same as the EIA/ISO program but with certain differences as shown below.
1. In the manual program machining unit, 1 line of tool sequence data corresponds to one block of the EIA/ISO program, which limits the number of data which can be entered in one block. (G: 2 data, S: 1 data, M/B: 1 data, Others: 6 data)
2. In the manual program machining unit, the tool is deviated on a distance entered in the article ACT-φ on the TOOL DATA display (on the nominal diameter in case of the data absence) when the tool diameter correction command (G41 or G42) is given.
3. In G98 mode, value of F cannot be entered with a decimal point. If the method of feed is modified from G98 to G99 or from G99 to G98, the designated feed value of F in the unit data will become blank (****).
4. A MAZATROL program cannot be called up by the use of a subprogram call such as G65.
5. Do not enter G109L for G1 or G2.
6. Do not use address P (waiting) for DATA-1 to DATA-6.
Note 2: When a turning tool is selected for the manual program machining unit, the rotational direction of the turning spindle is determined by the rotational direction set in the tool data. For a milling tool set the rotational direction by the M-code.
Lastly, Mazatrol can be alternately created using "three digit G code". This is covered in the back of most mazatrol programming manuals and Data I/O has a "translator" soft key switch called "text output". Therefore you can create a mazatrol program, then output it in text only, and get an ascii text file full of incomprehensible 3 digit G codes! This text output can also input and can be used for parameter and tool data/offset. If you have an offline tool setter, which is usually EIA only, the ascii text "G10 L50" bizness can be used to get external data into the control. It's helpful capability to deal with external electronic devices that don't speak mazatrol, which is about 99.9% of everything out there! (Mazatrol can be thought of as User Macro programs on nitromethane, steroids, with the dial set to "11", while drinking Jolt Cola and smoking meth. It's invisible to the end user by design, but the 3 digit format allows you a little peak into the guts.)
Can you put 3 digit g code in the body of a G code program. or use 3 digit format in a mazatrol manual unit? Never tried it, but I strongly doubt it! And why would you want to, anyway?
Ask me what time it is and I'll tell you how to build a watch. (The CT Solidworks User group held their last meeting at the Bristol Clock Museum. Clocks are a lot more interesting than I realized!)
Okay, my bad, it is actually a Matrix control. I don't really think you understand my question. I want to know if I can use a Mazatrol unit, i.e.
Originally Posted by 90-percent
bar out, bar face, thread mill (or whatever it's called) to create a thread milling operation. What I think your saying is, it must be programmed line by line manually with G codes?
I thought at some point we covered this in our Mazak milling class. And since the Integrex is basically a lathe with milling capability, I thought there was a similar cycle on that software? Maybe like tornado threading? Sorry, it has been a few years since we studied this subject. thanks,
I completely missed your "for thread milling". I thought you were talking about something completely different! My bad.
There is indeed a tornado milling cycle that was in place in at least the Fusion, if not earlier, for Mazak mill-turn machines. Now, I'm getting info bleed between machining centers, mill-turn fixed turret and Integrex mill turn, so bear with me. (Isn't there even another synonym Mazak uses when dealing with helical tool path?)
Here's what I have down good - Point machining - tapping, the trick is to switch on "tornado" in the line at the top of the unit defining tool and process. Then the tool data should have a switch for floating or fixed for tap tool.
Point machining - circle mill - has a poorly documented trick where you use the number "0" in the field for 1-9 surface finish designation. This forces the circular milling to stay in helix for the entire circular cut. The 0 has to be keyed in, it is not in the softkey selection set! If this is not 0, then when depth is reached it does a full 360 degree clean up, as it thinks it's driving an end mill generating a flat bottom.
The funky thing about thread milling in mazatrol is that the cutting tool will go into the hole at least one revolution (which is one full pitch) plus some additional parameter fudge deeper than necessary, and then enter the cut in a Z plus feed direction for the milling cut. (So the tool path would be ccw for a RH thread, yes?) It does enter in a small 180 degree arc that is approximately half the radius of the circular tool path.
Another thing is that it appears to be intended for a milling tool with only one (thread form) tooth. Therefore you have to use some false numbers for your Z depth if you have a common garden variety multi-tooth thread milling tool and only want to make one revolution in your cut. If you do it 'correct', Mazatrol will make as many revolutions as it would take for a single tooth cutter, so if you have a 1/2-20 and the hole is 1" deep, it would do 20 360 degree rotations to generate the thread!
Now it gets hazy - In tool data, do you name the tool a tap or a milling tool? (there is no such thing as a thread mill in mazatrol-land) Is there some oddball stuff depending on your plane selections and tool orientations? (can you helix in X-C plane for example?)
One tip that may help put the puzzle together is that on MATRIX Integrex milling/driven tools, the Z axis is always with respect to the rotating tool centerline, at least in Tool data. And X-Y is also to the tool, instead of the machine axes. I think this concept bleeds into when you program any unit that required a B angle input (which is virtually EVERYTHING on an Integrex!)
CUT A LOT OF AIR! And a lot of single step tool path check! More hints and clues are possible if you look at the TPC page for your unit and glean what tweakable parameters are allowed. And this may get you more optimization if the 'stock' mazatrol doesn't quite work as good as it should.
I write short stories instead of concise business writing. Sorry.
One more thing
Unless it was developed in the last 18 months and I wouldn't know about it, thread milling in mazatrol acts like something of an afterthought. You can do it in Mazatrol to an extent, but it takes a lot of mastery and fore knowledge to use it at all, and it can't do blind holes or O.D. threads.
The EIA only user macro's you can download from thread milling cutter people
apply to a lot more possibilities than the restrictive mazatrol way.