lathe cutoff suggestion

[Sbarner]

Hi All,

 

I have a suggestion for lathe. I don't know how you guys in industry cut parts off, but here, we part things off with some material to backface. We don't have a sub-spindle so the back facing is a separate operation later. When I setup geometry for a cut off operation, I generally draw a point on the corner that I want to part off, then translate the point in -Z by whatever meat I want left on it. It would be SOOOOOOOOO nice to be able to pick the corner I want to use, then have some parameter in the dialog to "Offset Z Coordinate" or something along those lines. This would be a huge time saver for those of us who part things off like this.

 

I know, I know...I can simply enter the position as a hotpoint, but after dealing with the lathe package and all its.... *...clears throat...* splendor, I just want to have a nice easy way to make the boundary point. Perhaps I'm missing something? Is there a way to do this currently?

[Sbarner]

Another suggestion. How about being able to choose if I want the retract peck moves in cutoff to be rapid or feed moves.

[chris m]

quote:

---

Is there a way to do this currently?

---

I offset a line .015 or .030 from the part and pick that...oh, yeah, that's what you said

 

 

quote:

---

How about being able to choose if I want the retract peck moves in cutoff to be rapid or feed moves.

---

How about being able to select a feed-only option in grooving in general? I can't tell you how many programs I've needed to edit because the little .039W grooving inserts can't survive a G00 out of the groove when they're touching the walls on both sides. 2 different feeds for full-width and step-over passes? 1st plunge diameter in facegrooving?

[Goldorak]

Very EZ , tell mastercam that you use a .150 part and put a .125in the machine, so it will partoff with a .025 over stock for the second operation, no need for extra geometry. just click the backside of your part when cutoff operation ask for a reference point

 

in lathe , you have to lie to mastercam to get things work properly

[Dave.L]

I don't use lathe yet but I assume it does not have a field like "stock to leave on face" kinda like mill "stock to leave on walls/floor"

 

[Goldorak]

^not in cut off operation

[Dave.L]

quote:

---

^not in cut off operation

---

I sure hope it is there for other operations.

 

I use this feature in mill for plating allowance and grind stock all the time....

[Goldorak]

yes we got stock to leave in any other turning operation

[G10X0Y0Z0]

no lying to mastercam here ( if you have to lie to the software then you might not be using the software properly )when mastercam asks for the geometry, push the space bar and type your Z & D cut off position. eg if my part is 1.00 dia X 2.00 long i D1.05Z-2.025 and set my cut off parameters. mastercam automatically creates th cut off point for you. the point can be moved at this time in either the Z or D.

[chris m]

I never tried that; good tip. I will check it out the next time I have a cutoff op.

 

As far as this goes:

 

quote:

---

if you have to lie to the software then you might not be using the software properly

---

That is total BS. If you use Mastercam Lathe regularly and don't have to create fake geometry from time to time, extend lines or chains that don't need to be extended, create "fake" tools to cut on one side or the other, then you're using some special unreleased version nobody knows about.

[Roger Peterson]

parting - When selection my cutoff point I use relative to the corner of the part and punch in Z-.025 or whatever I want.

 

grooving, both the roughing and the finishing portion of grooving has an option for outputing retract moves as a feedrate which you can specify. The only rapid moves are then transitions from one finish pass to the next. Unless I'm not understanding what your looking for.

 

The majority of geometry creation can be avoided by using the extend contour feature in lead in/lead out and by using the adjust stock function. Don't forget you can dynamically slide your start and end points of your chain. But yeah, sometimes you just need to draw a little geometry. And having two tools that are identical so you can have CW and CCW rotation is a limitation of the tool types we have available, until we get a a single tool that can be used for drilling, ID turning, and OD turning it's a pain.

 

Definately send in examples so they can see what and why you are looking for different functionality.

 

JM2C

[Philcott]

There are a number of ways to get mastercam to leave an amount for facing on the next opp but wouldn't it be nice to simply have a field where you put in the amount to leave? I know I'd prefer that.

 

It would be so simple, make it like facing. Pick the corners and set the amount and done. Why not give cut off the same feature?

[chris m]

quote:

---

Definetely send in examples so they can see what and why you are looking for different functionality.

---

Not to be a total downer on the Lathe product, because it makes us a lot of money, but we've had huge threads on this website, started by CNC Software reps, that have essentially been ignored. We've been waiting for multi-spindle, multi-turret support for years, and many of the simplest functions have been ineffective or required workarounds forever.

 

You are, however, correct about the feedrate in grooving retract moves; I just got so used to b!tching about that that it stays in my mind now.

 

C

[Sbarner]

quote:

---

The majority of geometry creation can be avoided by using the extend contour feature in lead in/lead out and by using the adjust stock function.

---

Evidently, the extend or shorten contour fields are not active in the cutoff operation. That would be a nice workaround if Mastercam let you use it.

[Sbarner]

Also, how about a parameter to change feeds and speeds in the facing toolpath to accommodate roughing AND finishing. It's so dumb to make an operation to rough face material and then have to make a completely separate op to simply change the feeds and speeds for the remaining .015" of material. I know this can be done. We have that option in mill with 2d pockets.

[Philcott]

quote:

---

push the space bar and type your Z & D cut off position. eg if my part is 1.00 dia X 2.00 long i D1.05Z-2.025

---

Nice tip that I will use from now on.

 

quote:

---

I never tried that; good tip. I will check it out the next time I have a cutoff op.

---

I program my lathe in the D+Z construction plane. I had the plane change on me when I tried using this tip but was able to get it back to D+Z and then put in the values needed.

 

That said, what a simple little annoying thing it is to have to do this in the first place. "Stock to leave" would rule here.

[tryon]

typically the cutoff tools in all our lathes never get taken out. So they are already offset in Z to leave the desired amount of stock. So not really an issue for us. But i agree it would be nice to have a "stock to leave" for this.

[Josh Kinney -Elite Engineering]

I 100% agree with all suggestions here.

[Eric E]

Here is how I do cutoff operations

1. Create a point at the intersection of the longest Z & largest X

2. Then transform that point in Z to add stock

3. Choose cutoff toolpath and select the created point as the boundary point