OT:Tooling and horizontal programming off CL of rotation

[cobra95kev]

What method do most of you guys use for programming horizontals? I like to program off CL of rotation and post the code all with one offset

to the location the part is at. The problem we are running in to is we don't have standardized tooling and sometimes the part doesn't always end up in the same location everytime we go to run the part so we have to turn around and repost the programs for the new location. Problem is this is taking up alot of my time and we are hoping to find a better way.

 

I had heard there are some calculators out there that can calculate offsets for parts that have odd angles (other than 90,180,270,0)

 

How do those work and would that help us in this situation?

 

Any help would be appreciated.

 

Thanks,

[Mgrenier]

Kevin,

 

We have made a custom macro for our machines so that the machinist can place the part anywhere on the machine and everything works great.

 

Can't share the program but am can answer all of your questions if you need.

[Tim Johnson]

I use just one offset (found at B0) and run a coordinate program to create new offsets at each plane change and uses G59 for the new offset.

 

This is an M-code program (G201)

code:

---

%

O9018(G201 -- XZ COORDINATE ROTATION PROGRAM)

(PARAMETER 6058)

#10=[13980+[#4130*20]](CURRENT FIXTURE OFFSET NUMBER)

#11=[#10+1](NUMBER FOR CURRENT OFFSET X)

#12=[#10+2](NUMBER FOR CURRENT OFFSET Y)

#13=[#10+3](NUMBER FOR CURRENT OFFSET Z)

#14=[#10+4](NUMBER FOR CURRENT OFFSET

#15=[ABS[#921]-ABS[#[#13]]](Z LENGTH FROM PALLET CL)

#16=[#[#11]](X LENGTH FROM PALLET CL)

#17=SQRT[[#15*#15]+[#16*#16]](HYPOTENUSE LENGTH)

#18=ATAN[#16]/[#15](ANGLE FROM PALLET CL TO PART ORIGIN)

(NOW MAKING NEW G59 COORDINATES)

#19=[sIN[#18-#2]*[#17]](PART ANGLE + ORIGIN ANGLE X LENGTH)

#20=[COS[#18-#2]*[#17]](PART ANGLE + ORIGIN ANGLE Z LENGTH)

#5321=[#19](X G59 COORDINATE)

#5322=[#[#12]](Y G59 COORDINATE)

#5323=[#921]+[#20](Z G59 COORDINATE)

#5324=[#[#14]](B G59 COORDINATE)

M99

%

---

#921 is the distance from the spindle nose to the center of the pallet at machine home. Also this is setup for the 300 offset option. A snippet of how I use it;

 

code:

---

O4221

(NO.4 CENTER DRILL 0 DEGREE SIDE)

IF[#153EQ#0]GOTO1

N13520 G00 G90 X.69 Y.36 B0. G54P[#900+1]

N13530 G43 H17 Z2.765 S8404 M[#933]

N13540 G99 G82 Z2.442 R2.765 P8 F50.42

N13550 X-1.31

N13560 X-3.31

N13570 X-4.26 Y2.25

N13580 Y4.25

N13590 X-3.31 Y6.14

N13600 X-1.31

N13610 X.69

N13620 X1.64 Y5.25

N13630 Y3.25

N13640 Y1.25

N13650 G80

N13660 G00 Z10.25

(NO.4 CENTER DRILL 90 DEGREE SIDE)

N13670 G91 G00 X0 G54 P[#900+1]

N13680 G90 G00 B90. (<<<<<<<<<<<<<<<<<<<<<<<<<)

N13690 G201 B90. (<<<<<<<<<<<<<<<<<<<<<<<<<)

N13700 G00 G90 X.495 Y1.375 (B90.) G59 (<<<<<<<<<<<<<<<<<<<<<<<<<)

N13710 Z2.1

N13720 G99 G82 Z1.777 R2.1 P8 F50.42

N13730 X-.13 Y1.25

N13740 Y5.25

N13750 X-.755 Y5.125

N13760 G80

N13770 G00 Z5.75

(NO.4 CENTER DRILL 180 DEGREE SIDE)

N13780 G91 G00 X0 G54 P[#900+1]

N13790 G90 G00 B180. (<<<<<<<<<<<<<<<<<<<<<<<<<)

N13800 G201 B180. (<<<<<<<<<<<<<<<<<<<<<<<<<)

N13810 G00 G90 X11.23 Y3.25 (B180.) G59 (<<<<<<<<<<<<<<<<<<<<<<<<<)

N13820 Z3.77

N13830 G99 G82 Z3.447 R3.77 P8 F50.42

N13840 Y1.5

N13850 G80

N13860 G00 Z11.25

(NO.4 CENTER DRILL 270 DEGREE SIDE)

N13870 G91 G00 X0 G54 P[#900+1]

N13880 G90 G00 B270. (<<<<<<<<<<<<<<<<<<<<<<<<<)

N13890 G201 B270. (<<<<<<<<<<<<<<<<<<<<<<<<<)

N13900 G00 G90 X2.63 Y1.25 (B270.) G59 (<<<<<<<<<<<<<<<<<<<<<<<<<)

N13910 Z12.08

N13920 G99 G82 Z11.357 R12.08 P8 F50.42

N13930 X2.32 Y.75 Z11.735

N13940 X-.68

N13950 X2.32 Y6.25

N13960 X-.68

N13970 X-2.37 Y5.25 Z11.357

N13980 G80

N13990 G00 Z15.75

N1 M99

---

[cobra95kev]

Thanks for the tips guys,

So how do you setup your part in MCX?

Do you just put it right on CL at B0?

I think this is a little over my head. Is there anything I can read up on kind of like an idiots guide to using this stuff?

 

Thanks again,

[Tim Johnson]

My zero points are set off the part (or fixture) wherever that may be. Most of my programs are used with Kurt clustertowers and the zero point usually comes from a corner of the material . The snippet I posted came from a dedicated fixture with the X,Z coming from the center of a pin and the Y from the fixture base. The pin is approx 5" offcenter in the X and 1" off in the Z.

[Larry Metzler]

Tim, reading your reply, brings up a dissicussion we are having at the present time at our shop. We are new to 4th axis programming and at the present time there are two trains of thought. At the present time the way we work is around a template tombstone that has been created around the machine WCS, At the time of programming we place the part on the tombstone (any given place in the working envelope). The work offset is then located

from a given point on the work piece, this is normally X Y Z zero with B 00 (G54 P??). The machinist will indicate the given point off the part. If the work piece is rotated ( B90), a new zero point is set from the new face and this will become G54 P??+1.

The WCS always remains the same, all programming is done by creating new construction and tooling planes, which are assigned new work offsets.

It was mentioned that if all machining was programmed from the centerline of rotation there would be no need for multiple work offsets. Is there any advantage to working this way?. I am not sure how this would be accomplished and it would seem to me to create more risk, with a bigger chance of error than the present system we use. I would appreciate input and advice from anyone who is more familiar with 4th axis work than we are at the time. Thanks All!

Larry

[Guest]

have worked it both ways for many shops. both work well if standards are followed.

 

center line of rotation programming makes modular tooling a must. your part must always load in the same position or you must repost program. reposting a programming is like starting from scratch and presents more variables than needed in my opinion.

 

calculating from center line to zero point on part works as well. but when programming you must always use that point for your tool plane zero.

having much hands on setup 4 axis experience this is my preferred method as i can easily calculate and follow the numbers as they relate to the drawing. if your set up persons cannot do this its a wash on wich method.

 

doug

[MIKE C.]

I have ran 4 axis horizontals for years and have been programming them for a couple of years.

At my old job we used chick vises and alot of technigrip tombstones.and programmed everything off of center of rotation and we used the expanded work offsets in the control so that the operator could fine tune any missmatches This allows the operator not to have to set xo yo zo every time and saves alot of setup time.

(if you dial your tombstones in on center of rotation you will have no problems with missmatch or repeatability).

i am currantly at a shop that uses kurt vises and i have found that if you set your xo yo zo off of material in jaws you cannot program it as a 4-axis unless you get the dimensions from the operator on where the material actually is on the machine and then you don't know for sure where it will be exactly the next time you set it up. The chick vises are expensive but will pay for themselfs very quikly.

programming from the center of rotation is the only way to go in my opinion.

if you are currently just starting to get horizontals, i recommend that you start programming from center know instead of waiting until later,it will save alot of time and money.

one more thing i would set it up so that you program everything from B0 and have a subprogram so the operator can change his B-rotation to what ever side he is going to set the part up on.

[Tim Johnson]

quote:

---

i am currantly at a shop that uses kurt vises and i have found that if you set your xo yo zo off of materiali am currantly at a shop that uses kurt vises and i have found that if you set your xo yo zo off of material in jaws you cannot program it as a 4-axis unless you get the dimensions from the operator on where the material actually is on the machine and then you don't know for sure where it will be exactly the next time you set it up. you cannot program it as a 4-axis unless you get the dimensions from the operator on where the material actually is on the machine and then you don't know for sure where it will be exactly the next time you set it up.

---

If your programming your xo yo zo off of material in jaws you shouldn't CARE where it is in the next setup (within reason of course). In our clustertowers as long as they're using the correct parallels they can be up to 1/8" off in their location and still not miss a beat. Any further off than that and they may be machining vise jaws but they'll be machining them to size.

[Guest SAIPEM]

Try this.

 

http://www.cncci.com/products/Fixture%20of...0calculator.htm

 

http://www.cncci.com/resources/tips/hor%20...al%20origin.htm

[MotorCityMinion]

Larry, there is a HUGE advantage to working this way. No reprogramming and no trig work the next time you run the job. Also, tool lengths, relative to the spindle nose and in set-up sheets remain the same if you place the part in the same location at every run. If your running multiple pallets, it gets even easier when you locate off center of rot. A lot of peeps have trouble grasping this concept if it's there 1st time around with horizontals. Heh, some never do, and others can't even rotate the part other than in 90. deg. increments.

[Dave Ball]

Just wondering how do you guys using COR handle second or multiple operation parts? How do you get the detail cut in Op2 to "line up" with Op1?

[cobra95kev]

SAIPEM,

 

Thanks for the links, I think we may end up going that route.

[Charlie Pierson]

IMHO

Programming a Horizontal from the center of rotation makes as much sense as programming a Vertical from G28(zero return) or, better yet, programming it from the pub in the next town over.

 

If you have fixture offsets and WCS offsets, why not use them (G54-G59)(G54P1-G54P48)??

 

We program from a logical part zero then that zero is described in G10L2 or G10L20 blocks (our WCS offsets).

If the part gets rotated we use another WCS. from either the same zero point or a new one that makes more sense.

 

For example: Top Cplane=B0 -> G55, Front Cplane=B270-> G56, Back Cplane=B90 -> G57, or whatever you need.

 

In other words , each rotation point of the tombstone is treated like a mini-VMC.

 

We also use positive Height offsets which are actually the length of the tool from gage line so we can share the tool thru different tombstone positions or different jobs. (tool is measured offline)

 

No re-posting needed unless the engineers alter the topography of the part.

 

Keep It Simple.

 

cp

[Tim Johnson]

MotorCityMinion,

 

What do you do when;

 

the fixture gets reworked?

 

the job gets run on a different machine?

 

the material came in undersized but is still useable with an offset change (due date in two days)?

 

the material was cut crooked so you need to clamp 1/4" max to keep the part from "squaring" itself.?

 

Stuff like this happens often enough here and I usually won't hear about it and have no need to. They just set the one offset per part,push the green button and let the program take care of the rest.

 

Edit: Charlie, check out the m-code program. You only need one offset per part (and one temp offset total) no matter how many plane changes you may be using. I don't know if you run multiple part fixtures (I would suspect you do) but you can run 48 different parts if you have the 48 work offset option.

 

[ 02-29-2008, 04:13 PM: Message edited by: Tim Johnson ]

[Guest SAIPEM]

Charlie,

 

The simplicity of using Center of rotation is this, you have one central reference point, ALL Work Coordinate offsets start off using the same point.

This means any adjustment to the individual work coordinate offsets are small incremental changes.

 

This method is the preferred method for anyone who uses probing.

 

It's also the most efficient for parts with multiple angular features.

[Tim Johnson]

SAIPEM,

 

I'm thinking your the idea of "Center of rotation" is different than the generally used description. When I hear the words "Center of rotation" I think of only one work offset being used and locating the pallet "zero point" to run one or more parts in a program. I don't consider what I do as programming from the "Center of rotation" though what I do would definitely fit your description.

 

I don't think probing has anything to do with what system you use though.

 

Using your description I would have to agree with the effciency.

[crazy^millman]

Charlie I will be the person to disagree 100% with you on this front. The way I program center of rotation is from center in X and Z and Y can float. I most times was programming parts that had 4 to 8 indexes being done on one side. Your method requires to much work IMHO. The idea of making fixtures and set-up is to not have to re invent the wheel everytime you set-up a job. With a correctly mapped tombstone, repeatability should never be a problem. Come to think of it I did a part that was full 4th axis milling and maybe close to 50 indexes in one part. Your method would have me using 50 workoffsets how efficient is that for running a machine. I can only imagine the set-up sheet. Now for index angle 4 deg your work offset is G55 for angle 8 it is G56 for angle 16 it is G57 and so forth till you are G54.1P48 and still have maybe 10 more indexes to set-up. Not a good way to approach 4th axis programming vertically to horizontally for that matter. Again just my opinion here.

 

The Kurt vice program is solved by using soft jaws and milling a skin cut. Now that should repeat if it does not then need to check those vices. To each their own and not trying to be against you here Charlie, but I have never liked one way of doing somethings on a machine and another way of doing other things and your way makes some one program parts all types of different ways when more than simple indexes become involved it also lends itself to not thinking outside the box when programming and setting up part on a machine that in 2 operations should produce completed parts 95% of time. I have seen many parts that were 6 to 12 operations on a vertical get done in 2 on a horizontal. Maybe a little harder to set-up, but when you cut 4 to 10 set-ups and 4-10 chances to scrap a part off, well worth the time to get it done right and save money in the long run.

 

Just my thoughts on this subject.

[Guest CNC Apps Guy 1]

I personally like programming for CL rotation. There's more benefits that drawbacks from my experience.

[Larry Metzler]

I want to thank all of you who took the time to

reply to my question.While I am not sure which

way is correct, it has opened my mind to the

opinion that programming from the C/L of rotation

must certinly be something we will have to look

into.Again thanks all.

[mowens]

The only way I have ever programmed horizontals, and I have programmed quite a few, is by setting my machining axis at the center of rotation of the table. I wouldn't want to do it any other way. But, like it says in the links referenced above, your tooling has to be dead nuts. However, that has never really been a problem. If you design and machine your own tooling, and you have a 2 inch grid pattern on your tombstone, and a very accurate model of your setup, your good to go. Just be sure you retract far enough not to crash when you rotate B axis.

[YoDoug®]

quote:

---

or, better yet, programming it from the pub in the next town over.

---

I am interested in learning more about this style of programming, it sounds more enjoyable than my office.

[crazy^millman]

One last thing I will add to this subject program a pallet pool system from anywhere you want and see how quick you run out of work offsets or program all of your pallets from center of rotation and see which way yields the best results. Sure is sweet when you can have 200 tools in a machine call 14 different pallets all using the same fixture offset and make good part without the operator having to re-pick up all of those offsets because you did not think far enough ahead to make it that way programming from different places in space on a tombstone verse having everything made correct from the get go so it would repeat and save tons of set-up time switching between job to job.

 

A little more thought on this using G54 to G54.1P48 you should in my thinking have a machine work for you not you working for it. If you have 100 different jobs and require 100 different work offsets to set them up how much time are you taking setting up all of those jobs? If you have 100 jobs all using the same workoffsets how long does it take to set up those jobs??

 

Every run a CNC lathe for anyone not sure if programming for center line is the correct way or not? Do you everytime you put a drill in a lathe have to sweep it in or just load it touch off Z and run it?? If you indicate drills in everytime you are wasting time you are not using the machine to do the work for you. If everytime you are putting fixtures and parts in a Horizontal and having to figure out where they are then to me you are wasting time making it harder than it has to be.

 

Again these are my thoughts on the subject and more than willing to listen to better ways of Manufacturing, but the question is are you??

[Craig Madsen from CM3D]

As long as you are only using toolplane programming then the macros to calculate position and update a WCS at the control will be good.

 

As soon as you want to do simultaneous axis movement you need to have your part drawn where it REALLY IS in Mastercam.

[MotorCityMinion]

Flame suit on.

 

What do you do when;

 

the fixture gets reworked? MCM: re-work it properly.

 

the job gets run on a different machine? MCM: Post to the new machine

 

the material came in undersized but is still usable with an offset change (due date in two days)? MCM: Issue a NCR to purchasing then grab some shims.

 

the material was cut crooked so you need to clamp 1/4" max to keep the part from "squaring" itself.? MCM: Change saw blades.

 

 

Nubs. Centerline of rotation is the same on any machine, which BTW, does in fact allow a programmer to program from the pub across the street. If your operators can actually put a fixture where it belongs, it will work on any machine, just change the post. Of course I'm talking about programming real work, with multiple planes on it in increments other than 45. and 90. deg, not the rough sawn raw material that any noob could run on a Bridgeport.

 

Did I make it through the interview?

Time for a brew. Join me across the street before the center of this pub starts to rotate.