Z setting in lathe programming

[MultiAxGod]

I have a need for you guys' response for an in house debate on where to set the Z0 for lathee programming.

In all of my experience, Z0 has been the face of the part at finish. Regardless if you are roughing or finishing. The set up sheet and notes reflect how much material if roughing is to be left. The machinist then sets his tools to be at Z0 for the finish face of the part. If you are leaving .03" on the face for a finish operation, the program shows a Z value of .03".

How do you do it?

[BrianCNC]

That is how I have always done it.

[Mike-T]

Same here.

[Guest]

I've done it like that 98% of time.

 

The rest of the time was fixture work that had a location point, so that point was used.

[MultiAxGod]

Thanks Brian, Mike and JParis, I need more people to input!!! I agree about the fixture work also! C'mon CNCApps, Hardmill, Crazy! I need lots of input on this one!

[chris m]

I would say that 99% of our lathe programs, and we have thousands of them, use the finished face of the part as Z0. Sometimes it is easier for setup to use the stock location surface, particularly if you are machining a lumpy casting, or if you're doing secondary machining on something that doesn't have much surface area on the face, because touching off can be difficult. The only time that I require programs to be generated with Z0 at the stock location surface is when the part will be flipped around and re-chucked in the same program; zero shifts in your program are a recipe for disaster IMO and machining your second side referencing the face on the first side just doesn't make any sense to me.

 

C

[[email protected]]

Same here

[Tim Simmermon]

Z0 = Finished Face for us as well. If we are flipping the part within the program, we set G54 for side one and G55 for side 2. G55 would also be set at the finished face for that side as well.

[generaldisarray]

Same here.Then when you scan your file before sending it to the machine if you see Z- you know you are in the danger zone.

[Philcott]

Z zero is almost always the finish face of the part.

 

quote:

---

The only time that I require programs to be generated with Z0 at the stock location surface is when the part will be flipped around and re-chucked in the same program; zero shifts in your program are a recipe for disaster

---

We use this process on occasion and on a rare occasion we use different workshifts when flipping a part.

[robh]

Z0=finish face here too

[MultiAxGod]

Hey general, you don't work at Creative Blow Mold do you?

[Goldorak]

quote:

---

Z0=finish face here too

---

same for 99.9% of our programs

[Jmick]

same here

[JPensack Acker Drill]

Finished face of the part is Z zero here on all one side programs. On turnarounds we set our first side zero as .09, so that when we flip the part the finished size is Z 0. This means that all Z#'s on the first side are +.09. We have all Okuma lathes so we don't have the G54, G55 ability, but we haven't had any problems yet.

[X-L Engineering Corp]

Thats how it's always been done here

[chris m]

Your Okuma lathes can easily do the same thing as G54, G55. If you always have the same shift amount [like .090] then you can put this in at the beginning of the second side:

 

V1=VZOFZ (saves first side zero into common variable)

V2=V1-.090

VZOFZ=V2

 

You could, I believe, do this as well, I just don't like referencing the same value on both sides of the equation:

 

V1=VZOFZ (saves first side zero into common variable)

VZOFZ=VZOFZ-.090

 

 

Then, at the end of your program, shift it back to the first side:

 

VZOFZ=V1

 

If you don't use the same value all of the time, put the value in at the top of the program as a local variable like this: SHFT=.09

 

Then use:

 

V1=VZOFZ (saves first side zero into common variable)

V2=V1-SHFT

VZOFZ=V2

 

User task rocks!We build our zero position in the program [spindle face+height of chuck+distance part face from chuck=Z0] and have never had an issue with it

 

POFP=5.0270 (PROJECTION OFF FACE PLATE)

.

.

.

VZOFZ=V182+V183+POFP

 

In this instance V182 is the spindle face, V183 is the thickness of the faceplate, POFP is the distance from the faceplate to the part face

[Guest CNC Apps Guy 1]

I've used 2 methods. One, most everyone here is in agreement with, the other method I've used is the spindle face. I've always liked having a fixed point for everything. But for all intents and purposes, probably 90% of the lathe programs I've written was to finished part.

[gcode]

I write programs for big VTL's ( up to Ø30 feet)

Z0 is usually the surface of the part that rests on the fixture or table

On some complex castings Z0 may be some datum plane so the machinist can read dimension off the blueprint..very rarely is the finished face Z0

[MultiAxGod]

THank you gentlemen, I appreciate the input and feedback.

[calnet42]

Most of the part I program now are from 15" to 40" dia and we almost always use the location face as the Z zero.

It allows the operator to set the tools directly off the fixture or the jaw face.

It also will let the operator look at the operation sheet and find the finish face dimensions in the program directly with no math needed.

 

At my previous job, I worked on parts from .100" to 10.00" dia and we usually used the finish face of the part as z zero.

[Charlie Pierson]

Like GeneralDisarray said.

[Columbo™]

quote:

---

Z0 has been the face of the part at finish

---

Same here