Lathe ID Tools make crazy moves

[chris m]

Good Morning Folks

 

I have been scratching my head about some of these oddities for awhile and just had another one so I figured I'd throw it out to you guys; anybody else seeing inexplicable rapid death moves on their ID toolpaths?

 

For instance, I am programming a part with an ID groove and I want to use reference points for safe approach / retract of my tool without creating extra geometry. When I place the approach ref point .100 in front of the part the tool comes into position as it should, then promptly rapids in the +X outside of the part, -Z over the top of the part, then right down thru the part to get to the start point of the groove path.

 

It will do this with the ref point set .250, .375, .500 in front but if I set it to .750 in front it starts to work right.

 

WTF?

 

V9.1 no service packs at the moment

 

C

[CNCGUY]

Are you using stock boundries?

[Brendan P]

quote:

---

For instance, I am programming a part with an ID groove and I want to use reference points for safe approach / retract of my tool without creating extra geometry.

---

Not trying to be a smart a$$ Chris,but I don't use ref. points on lathe very often.

I set my lead in/lead out entry/exit vectors and never have a problem.

When you define your stock,Mcam should know where/where not to go.

 

Some of the times that I have used ref. points in mill...

I had some strange things happen in my posted code!!!

 

Sorry I can't help buddy.

[chris m]

Yes, Troy, I am using stock boundaries

 

Brendan:

 

1) grooving doesn't give you lead in / lead out

 

2) Reference points are nice for steering around tailstock, lower turret tools, fixtures, etc

 

C

[crazy^millman]

Chris that was one thing I liked about the Mazak Controllers was the TPC (tool path control) points you put in every operation no matter the operation to clear things.

[Philcott]

Morning Chris,

 

I sometimes get strange moves when using reference points as well. I have never had a path like you describe though. Often I put in a point where I want to make my approach to get around the oddities. Not perfect but it gets me on to the next job.

 

Phil

[chris m]

Phil we used to add points all over the place in older versions but with the new stuff the ref points are sweet. I know I can work around this, but I shouldn't need to. Just asking to see if you guys have seen this stuff. I figured that you, Troy, Brendan, and maybe Brent Wilkerson would be the guys most likely to have seen this.

 

Where's Trevor 'Lathe Boy' Bailey on this one?

 

C

[Nominal]

I use ref points in the lathe occasionally and never seem to have a problem. Maybe you could put and example of this up on the ftp. I'd look at it.

[chris m]

I put the file on the ftp as Lathe Death Move.mc9

 

T10 is the problem child. It works the way it is, but if you move the ref point closer to the part it goes crazy.

 

Take a look and see if it is something I'm doing.

 

Thanks

 

C

[CNCGUY]

Chris,

 

Your ref. points are set to absolute. The cutter is trying to go to dia. 0 before cutting. The back side of the tool is wiping out the stock (zoom out to see it). I changed to inc. and it works fine. I uncheck ref. points and seems to work good also.

 

Hope I'm not stating the obvious. HTH

[CR]

Hi Chris

The only thing a saw was your reference points for approach and retract

 

I changed D to 3.1 (.100 below id)and Z to +1.115 (.100 in front of the part) on absolute for both moves

It works fine.

 

 

Clement Cobos

[Philcott]

Chris,

 

I had similar results as Clement and changing the reference points to make the path work, but that doesn't explain why you were having the backside of the tool burnish the face of the part. Do you usually program out in front of "Z" zero? I wonder if this had anything to do with the error.

 

Phil

[Prism Engineering Inc.]

Chris,

in job setup you can set home position clearance moves to get the tool to retract to the outer edge of the stock profile while doing I.D. work.

hth, phil

[chris m]

OK, here we go:

 

Troy

 

The 'D' value in my ref points is unchecked so the value has no effect. If the file on the ftp has these checked then it is a mistake as the version I have here does not.

 

Clement

 

I put the 'D' value in there and, like you said, it works better. However, all of the other tools work fine without the 'D' values, WTF? Like I said, I have workarounds but that doesn't change the fact that this doesn't work right.

 

Phil C

 

This is a part-flip job so I program with the part location surface as Z0. No zero shifts to worry about this way. I trimmed the file before I posted it.

 

Phil J

 

Are you talking about tool clearance? If so, that doesn't do what I want; if not, please clarify as I'm not sure what you mean.

 

 

Am I to assume that this means that you guys have the same result (the tool wiping out the part) when you run the file like I had it with the ref point at Z1.115?

 

 

Thanks guys for looking at it anyway.

 

 

C

[CNCGUY]

I did notice whatever I changed in the ref. points, when I went back it wasnt how I left it. Must be deafult to check diameter.

 

Sorry I couldnt be more help, I thought I had your problem solved.

[Philcott]

Chris,

 

Your assumption is correct. I do get the same results as you when I move the reference point closer to the part.

 

Phil

[MACHINEMASTERG]

phil,

 

where did camdude go???

[MATSSMan]

Chris,

 

There are 2 options:

 

#1

Click on the Stock Update button on the tool parameter page for the operation, un-check 'From Job Setup' and set the tool clearance for rapid moves to .049

 

#2 Change the stock clearance for the groove roughing operation to .051.

 

Either of these will solve your problem.

 

The tool clearance value puts an offset contour around the tool during rapid moves which is checked against the stock/chuck/etc during rapid moves. At the start of the grooving operation, this boundary touches the stock if the groove rough stock clearance is the same as the tool clearance. This, in turn plays havoc with the tool collsion module, which tries to avoid this situation by applying different methods to get the tool to the start of the operation.

 

... and results in the crazy moves that you get when it fails...

 

I hope this helps you out.

[Nominal]

quote:

---

This, in turn plays havoc with the tool collsion module, which tries to avoid this situation by applying different methods to get the tool to the start of the operation.

---

That looks exactly like what it is doing. One other way to cause it to work properly is to check the box under the groove shape parameters that says use stock for outer boundary. Clicking that one box will cause it to work the way chris wants and he can set the z ref to anything after that and it will work.

 

One wonders what its using without that being checked

 

Good explaination Matss

[MATSSMan]

quote:

---

One wonders what its using without that being checked

---

Without that box checked, the software assumes that the stock is a line joining the outer corners of the groove. (Which it is, for rectangular grooves on finished diameters...)

[chris m]

Nominal, you're the man! The damn 'use stock' box does make it work properly.

 

Thanks for all of the help and suggestions, guys!

 

C

[Nominal]

quote:

---

Without that box checked, the software assumes that the stock is a line joining the outer corners of the groove.

---

That's what it supposed to do. But with the chained groove geometry I wonder how its dealing with the radii edge breaks. It must be making that line joining the outer corners from the tangent of the edge breaks and the verticle walls otherwise there would be no different between the use stock check box being toggled on or off.

 

 

quote:

---

Nominal, you're the man! The damn 'use stock' box does make it work properly.

---

Yeah but don't tell my boss that I spent 20 minutes playing around with that.