Multiple offsets in lathe

[JPensack Acker Drill]

I am programming a shaft in MCX3 turn, and I have several diameters that are plus and minus tenths for the tolerances. I was wondering if anyone programs parts like this with different offsets for each diameter. If so how can you get mastercam to do that within the same toolpath. This is how our old programmer programmed such parts, he programmed by hand the old fashion way. Also, does it need to be done like this, will the diameters act different compared to the movement of the offset?

[chris m]

There are a couple of ways that I go about this:

 

1) If the relationship between sizes is consistent [typically things turn smaller the closer you get to the workholding] then I just fudge the geometry so that I can run one offset because it is easier for the operator that way.

 

2) If it doesn't look like option #1 is going to work, I use double or triple offsets on occasion but I don't call an offset change in the middle of a toolpath because that is a crash waiting to happen when the operator doesn't look at the paperwork and 'forgets' to input TLO values for your second offset. If I am using, for example, T0101 for the front of the part and T0121 for the back, I will create a toolpath for the front section with a safe position [lets say Z.250] as a retract reference point, then I'll create another toolpath for the rear, with Z.250 as the approach reference point, and use T0121 for that.

 

Hopefully that helps; feel free to email me if you have further questions

[JPensack Acker Drill]

Thank you for the input, have you had problems with the diameters not staying relative to the amount of the offset change. Such as you move your offset .001 and one diameter moves the .001, but another diameter moves .002? I can see on an old worn out machine but what about a relatively new one.

[chris m]

Diameters reacting differently to offsets is not something I see a lot, but the amount of stock that is machined on a re-cut can vary quite a bit [3 or 4 tenths is quite a bit to me, just to be clear here] and that can often cause some major headaches when getting size during setup or after insert changes. We usually see this on parts that project out away from the workholding quite a bit or that have significant thickness differences in different areas; the tool pressure on that part can cause some minute deflection when machining small amounts of stock [DOC less than the TNR exerts significant radial pressure away from the tool tip] which makes the tool "take more stock" in one area than another. Even very rigid, new equipment can suffer from this.

[JPensack Acker Drill]

Once again thank you for your input.

[gcode]

quote:

---

Such as you move your offset .001 and one diameter moves the .001, but another diameter moves .002? I can see on an old worn out machine but what about a relatively new one.

---

This can be caused by the tool

being mounted off center.

The effect of an off center tool on

a large diamter is minimal, but it can be

drastic on small diameters.

[JerryBenoit]

I agree with gcode first check your centerline and try to keep from putting in extra offsets. However sometimes you may need to use more. If you do jmake sure it is well documented. I usualy pull off the part and change the offset or adjust the offset the amount needed via a macro or G10. The best method is pull off the part end the sequance and start a new one the machinist or operator then will note the offset change and is less likly to have the machine crash if the turret indexs to the wrong station.

 

I just finish programing a large shaft that had several diameter changes of .01 to .02 in mid section. Between each change there was a radius of 1.5" to 2.0". The part length is 112". I program it with 1 offset put as we went down the length I took a test cut on a section, sized then cut my way down the shaft.

[tryon]

If we have some fussy diameters like that we will add a variable to the X numbers.

 

X[.933+#510]

Z-.76

X[1.245+#511]

Z-2.5

 

Documentation is key. Use the tool offset to move them all and the variables to adjust individually.

[JPensack Acker Drill]

How much do you leave for your finish cut? The programmer at my shop that I am taking over for programs by hand. He will write a program that looks like this:

 

T020204

(1.5 Turn)

X1.5

Z-2.0

(2.0 Turn)

X2.0 T020205

Z-2.5

 

I've seen programs of his that have 5 or 6 different turn diameters or bore diameters all with offset changes on the x moves. I can't see how this is necessary since that is resolution and accuracy on a cnc. We have Okuma lathes and the tolerances are +/- .001 at most. They have been doing this for years and I can't see why.

[Chris Rizzo]

quote:

---

[DOC less than the TNR exerts significant radial pressure away from the tool tip] which makes the tool "take more stock" in one area than another. Even very rigid, new equipment can suffer from this.

---

huh, never thought of it that way, makes perfect sense though. The cutting force moves from axial to radial as doc approaches a theoretical .0000 depth. Perfect tangency between the tool and workpiece would be a 100% radial force vector. right?

 

Oh, I use diff offsets to control tight (+/- .0003) dia. shoulders at opposite ends of 10-12" shafts we turn. All machines cut a taper of some sort, and this eliminates chasing your tail trying to use a single offset.