[Joe.B]

I know this must sound insane, but if you have a moment, I'm wondering how others approach the following 2 choices for 4th axis work:

1. Touch the OD of the part & make that Z0. (And retouch them again for different sized parts).

-or-

2. Have all your tools set on the centerline of the 4th axis & use the work coordinate to type-in half of the part's diameter (which does not require touching-off every tool again because of a different size part).

Some advantages can be noted for option #2. As already stated, different OD sizes just requires the operator to type in (half) the diameter... AND it doesn't matter if the program is written off the OD or written off the center. If written off the center, the Z work coordinate is 0.0000, and if it is written off the top of the OD, he (again) just types in the value in accordance with the part's OD.

My apologies for bringing up such an elementary issue, but disscussions around this shop have sparked the question, "What do other machine shop mill-hands do?"

[fizzissist]

You are correct.

1. Touch off the OD and make that your Z0.
.....or...
2. Set a theoretical X0,Y0,Z0 in space.
....or....
3. Set your zeros to some feature on the part, fixture, or space that makes sense for the job.

I ALWAYS chose the easiest program zero for the specific job.

But for your jobs, it depends on how the part was programmed ( reflected in the manslaughter rate of your company's programmers), or some factor that is driven by design or fixturing. Maybe your blank parts vary all over the place...forcing a zero based on fixturing, or measuring a fixed distance from a fixture point.

In other words.....it depends. There's no fixed answer.

[Joe.B]

Thanks for your insight, fizzissist.

But I'm just wondering about simple, cylindrical parts chucked in the 4th axis. The part (in most cases) only has 1 OD or just has mill work on a single OD.
(An OD that doesn't vary but about .005" or so)

What does your group prefer to do with the height offset in such a case?

[Geof]

You need an "all of the above" choice for your poll.

When I am doing a one-off setup I will probably touch off directly to the O.D. of the part with all tools.

If there are several parts with the same O.D. I will probably do the same thing.

When I will be doing parts with different O.D.s using the same set of tools I will either touch off directly to the largest part. Or I will touch off to a reference point that is higher above the table than the O.D. of the largest part. Then when I do the different parts I will enter a Z value into the Work Zero that is the distance from the reference point (or largest O.D) down to the O.D. I am working on. Actually if they are repeat jobs this value will be entered from the program using a G10 command or a G52 command. The Z value(s) are all negative

I neverset the Z tool offset to the centerline of the 4th axis. The reason for this is that then the Z value entered into the Work Zero has to be a positive value. If a negative value is accidentally entered the result is the tool tries to go below the centerline which probably creates a bit of havoc.

When the value that should be entered is negative and a positive value is accidentally entered the tool stays well above the work and just machines air. This creates far less havoc.

[fizzissist]

What Geoff says is correct (he's always correct..), but I'd like to add...

If you're doing the programming, then you can program it however you'd like, if someone else in the shop is programming and not doing the operating, then a simple discussion with them would be advised.

Just like in 3 axis, I VERY rarely will program a part so any portion of the part extends up beyond my Z0. If for no other reason, I know if there's a minus in front of a Z position/move, then I'm in the part. It makes editing easier, and a little safer.

For 4th axis, I generally will set the Y0 (on my machine the X is on axis with the rotary axis) at the centerline using a known dowel or the rotary table itself, and the X0 off an edge of the part or the X-locating face of the fixturing..depending on the part and how I programmed it.

For the Z, I almost ALWAYS use the finished OD as my Z0. If the part has some OD material to be removed, it's just a caveat to myself that there's some extra material/clearance to allow for. For convention, I still know that if the Z is negative, the tool's possibly in the part, even if the Y value is beyond +/- the OD....just for peace of mind. Still got that toolholder in the equation.

[txcncman]

My methods also depend on the job. One of the factors would be how many tools, 3 or 18? This is another one of those things about machining that anyone that has not graduated to "real machinist" status can't really understand. There are multiple ways to do any number of operations. Which way is chosen will depend on skill level, knowledge, experience, and how they feel that day. Have a fight with the wife that morning? Do the job one way. Get your production bonus check that morning? Do the job another way.

Most machinists will make notes to themselves when setting up different jobs and will indicate to themselves what was most successful. Then when setting up future jobs, they will go back and review the notes for a similar job and usually use a similar process. I have one whole drawer in my tool box dedicated to these types of notes.

[mfgbydesign]

Depends...
Contouring "full 4th axis" origin NEEDS to be the centerline. Option #2.
Aircraft Engine Augmentor Case Machining
1989 programmed in APT hence the mockup (predates software verification, $100,000 part)

Indexing around the same part on the same fixture? Ditto. Option #2.
http://www.mfgbydesign.com/images/9mmMX3.JPG
Part required 12 index positions. Where is the top of the part?

Multi-part fixturing or multiple fixtures on the same part? Whatever locating surface is easy to pick up on the FIXTURE from each index position, not the part. Not Option #1 or #2.
http://www.mfgbydesign.com/images/hmc-4ops.JPG
http://www.mfgbydesign.com/images/N036-2.JPG

When to use option #1? Never (with few exceptions).

[fizzissist]

Ok, here's an example for you, 4th axis on a cylinder.

What's different, unusual, is that I had to program a rectangular O-ring groove on the INSIDE of a 8" ID cylindrical segment. Where SHOULD the Z0 go?

Pick a finger, any finger. Now I'll mix 'em up.

:cheers:

[Joe.B]

The attached blueprint is what I am asking about.
Nothing fancy or complicated in the least bit.

Let's say you: center drill, drill, then counter sink the 4 holes.
Pretend your tools are already loaded in the machine from a previous job.

When setting up this part: do you MDI up all 3 tools & touch the OD?

And then you go to another job with the same 4 holes... but the OD is 6" instead.

When you do that setup, do you (again) call up all 3 tools & touch them to set all 3 height offsets again?

[txcncman]

The attached blueprint is what I am asking about.
Nothing fancy or complicated in the least bit.

Let's say you: center drill, drill, then counter sink the 4 holes.
Pretend your tools are already loaded in the machine from a previous job.

When setting up this part: do you MDI up all 3 tools & touch the OD?

And then you go to another job with the same 4 holes... but the OD is 6" instead.

When you do that setup, do you (again) call up all 3 tools & touch them to set all 3 height offsets again?

It all depends on where YOU want the Z zero to be. YOU decide. And then YOUR programming has to match. So, how do YOU want to do this?

Do YOU want Z zero to be the OD of each part? Then set YOUR tools to the OD and write YOUR program accordingly.

Do YOU want Z zero to be the center line of all round parts? Then set YOUR tools to the center line and write YOUR program accordingly.

For myself, I try to program so that ALL of the clearance moves are Z+ and all of the machining moves are Z-. This means I won't usually program with the center line as the Z zero point. I will use the part OD instead as the Z zero.

[fizzissist]

No, nothing fancy at all.....but again....

How is the program written??????? Are the Z moves based on the centerline of the part or the OD?? You need to set your Z offsets relative to where the program dictates they should be. Remember, you're simply telling the control where the tool tips are...it knows what you tell it.

If your program has the Z0 at the centerline, then you need to "touch off" your tools to the centerline by either setting up gage blocks, height gage, or something to mimick the centerline..or touch off the OD and add the radius to the length/distance of the offset value.

More simple in this your case, have the program for this part using the OD as your Z0, touch each tool off the OD, set the offset into your control, and go.
For the 6" part, just touch off the tools to the smaller OD and go, assuming the same wall thickness.

For some reason, this seems to be more complex to you than it should be, and no offense meant at all....I go through this myself all the time...over analyzing... Begs the question....WHO is doing the programming???

Posting some code may help us understand what's going on.

[Joe.B]

I'd like to thank everyone for their responses thus far & also extend an appreciation out to those that voted.

I have just recently joined this cnczone community... my apologies for not providing some background or at least a small intro to myself. So, briefly, this is me:

After the military, I went to college & also began machining for a major oilfield company. I was taught how to setup & run various parts on a CNC mill. Eventually, I began programming. Then I added CNC lathes. For the experience, I also ran a manual mill & lathe but quickly returned to present technology.

I moved up several times (to different companies) & after graduation I moved up again. I have been very fortunate to work with hundreds of other fellow machinists & engineers in different environments on different machines/controls, cutting different materials/parts.

I've been in this industry for about 12 years now. I work in Manufacturing Engineering for a company with 64 CNC machines. My main function is programming & processes but I frequently deal with computer & machine networking as well.

In recent years, we have invested millions in implementation(s) for Lean Manufacturing Concepts. We are far from done. Accordingly, I am ALWAYS interested in what's happening, what's new, how to improve, etcetera.

Again, many thanks to those that have shared.