Lathe crashing problem

[Shawn Wentzel- Wenteq Inc]

We have noticed a problem, and I dont know if it's my post. On a lathe ID toolpath, if you do a finish cut or a thread cut and create another operation with the identical parameters, say as a spring cut, the tool wont retract out to Z0.00 before going home. The part and boring bar usually suffer.

[Guest]

Do you have stock defined?

[Shawn Wentzel- Wenteq Inc]

Yes always

[Philcott]

I like to use the Reference point option on the tool parameter page and set the Z to .100 absolute for approach and retract. This will make sure the tool clears the part.

 

That is if your part face is Z0.0

 

Phil

[chris m]

Ref points ref points ref points

 

always always always

[Paul Felger]

quote:

---

Ref points ref points ref points

---

I wouldnt dare turn without them

[Colin Gilchrist]

Yep, reference points are a must have for Lathe operations.

 

I always recommend to users that they create a point entity at a safe intermediate retract location for both the OD work and the ID work.

 

For example, you might have a point at X3.0 Z.1 for your OD work, and a point at X0.0 Z.1 as Phil mentioned above.

 

Also, look carefully at your lead in/out values. There are a lot of options in there to make sure you get the proper retract distance and vector direction.

[ATG]

I've turned in allot of scrap carbide before I learned where the reference point option was!

[chris m]

quote:

---

I always recommend to users that they create a point entity at a safe intermediate retract location for both the OD work and the ID work.

---

Unless you can't get away with only [1] intermediate point [and sometimes I can't, so I create points] I would recommend you don't create entities for this, using the Ref Point is much easier.

[Vegard]

Im bringing this thread back from the dead, but I have a related question...

Is there a way to set the default z reference point for all internal operations?

 

I tried to go to the operation defaults, but I cant do it from there.

 

Thanks in advance.

- Vegard Hamso

[JPensack Acker Drill]

If you go into the machine definition manager, and click on the axes button. (It's a criss cross of three axis at the top.) On the bottom left there is a home position and a reference position. This will let you set a default home position, id ref. and od ref. for each machine. I have had problems with this sticking though with lathe. With mill I've had no problems. If it works let me know cause I'm still confused about why it won't stick.

[gcode]

quote:

---

I'm still confused about why it won't stick.

---

If you set this from Files/Edit inside the Operations Manager, you are setting it FOR THAT FILE ONLY and the edit does not change your

hard copy of the Machine Defintion..

Permanent edits to the Machine Def should be done from Settings/Machine Def toolbar at the top of the screen..

If you are already doing that, I don't know why it won't stick.

 

[ 03-03-2009, 09:53 PM: Message edited by: gcode ]

[Vegard]

Thanks. exactly what I was looking for.