Need Help!- Profiling program failing

[Turk88]

We have a TL-1 and we have been trying to create a program with a radius on the end...like a pawn in chess. We have failed everytime trying to create a profile. We are trying to do it using the custom profiler generator (or whatever it is caalled)

We can't seem to get anything to work other than simple parts. Anything with an undercut or a radius, like a 3/4 ball fails miserably.

[flashno]

We've found similar limitations. The lathe profiling software, unlike the mill, doesn't give you the ability to create CW or CCW arcs, just rapid moves or lines. You CAN, however, fillet 2 lines.

Try creating the 3/4 ball shape as a square shape (3 lines), the length of the 2nd line (along Z axis) would be 3/4, then fillet the 2 intersections using something just less than a 3/8 rad. This won't give you a true sphere, but close to it. I think the remaining lines after filleting have to be at least as long as the tool nose rad. Only way to create a true spherical shape (so far) is in CAD/CAM, not on the control.

I'm hopeful Haas is working to improve the profiling software, it IS fairly new.

Ed

[Geof]

Originally Posted by flashno .... Only way to create a true spherical shape (so far) is in CAD/CAM, not on the control.....Ed

This is not entirely correct. Programming a sphere is relatively simple and is possible using G71 or if you want to push a few keys simply by direct coding all the moves.

[tobyaxis]

Originally Posted by Geof This is not entirely correct. Programming a sphere is relatively simple and is possible using G71 or if you want to push a few keys simply by direct coding all the moves.

I have done this all too many times. The trick is to use TNRC and make sure you have the correct GEOMETRIC info in the correct places.

O0001
G0G40G80G97G99
S1500M3
T0101M8
G0X1.125Z.1
G71P10Q20U.005W.002D.1
N10G42G0X0.
G1Z0.F.005
G3X1.Z-.5R.5
G1Z-.525
N20G40X1.125
Z1.M9
G28U0W0
M30
%

I did not program with SFPM but you get the idea.
On the Geometry page there will be a Tool Tip Designation, Nose Radius Designation, and Tool Location from Home to the Work Shift.
All these are needed to have a trouble free Zero Alarm run.

[flashno]

Originally Posted by Geof This is not entirely correct. Programming a sphere is relatively simple and is possible using G71 or if you want to push a few keys simply by direct coding all the moves.

Your're right, of course, you can do it with G code, without CAM - I was referring to the original question about creating the shape in the IPS profile creator software - can't be done, as far as I know.

Very often we use a mix of CAM, IPS & hand G code on our TL-2. While CAM is great and IPS is good, though limited, you're right to encourage folks to learn & understand G code. No limits.

Ed

[Donkey Hotey]

Originally Posted by Turk88 We can't seem to get anything to work other than simple parts. Anything with an undercut or a radius, like a 3/4 ball fails miserably.

How old is the machine & software? I have a June 2007 TL-1. Are you saying you can't cut a radius using the profile software? Are you looking all the way over on the right column? I'm going completely by memory here but:

• The profile works by stacking up a series of commands.
• The first command is usually defaulted to a rapid move to a start position.
• The second line is usually defaulted as a linear G01 move, feed rate, etc.
• All subsequent moves that you add are also linear moves, unless you go over to the right column and change them to G02 or G03.

I haven't tried making a pawn like you're suggesting but I don't see any good reason why it wouldn't work (except maybe not having the proper cutter).

Are you getting some kind of error? Is your final move point at a larger X than your start point? That's very important because it establishes which quadrant the lathe is cutting in. If that doesn't make sense, look in your manual at the different canned roughing/finishing cycles. This still kicks my butt with certain profiles--but I'm learning.

[Turk88]

The machine is brand new with the updated software. We got it about 4 months ago. I have tried entering a radius into the column all the way to the right and it never shows the proper profile that we are trying to create.


And yes, I amaware it can be G coded and I can do that, as well as using mastercam to do it...but I was trying to use the IPS and it has failed for certain profiles

[Donkey Hotey]

I just looked at my machine and for the life of me, I can't figure out how to get that first column to change to Arc. You're supposed to be able to change that to 2 or 3 (arc). Mine will only do 1 or 4. I must be doing something wrong with the lead-in moves or something. I'll look at it again later.

[flashno]

Originally Posted by Donkey Hotey for the life of me, I can't figure out how to get that first column to change to Arc. You're supposed to be able to change that to 2 or 3 (arc). Mine will only do 1 or 4.

You're not doing anything wrong. As I said earlier, the lathe IPS software can't create arcs (2 or 3), only rapids and lines.

Ed

[Turk88]

I noticed that in that software it asks for a radius if you want to add one. This radius is supposed to start at the end of the previous line according to the prompt. I can't get it to work and my boss is pretty mad about it.

I like Haas. I enjoy running their machines but I don't think my boss will buy another one because he sees to many problems with it.

[Donkey Hotey]

It's all coming back to me now.

Yes, the lathe IPS can do the G01 method with an optional Radius value (G01 programmed with specified corner rounding) but it can't do non-tangent arcs like the head of a pawn. I wonder why they left the 'arc' prompts in there? I've been over this before and those prompts confused me yet again.

[Turk88]

I don't get why they will not allow this. Profiles like that are very common. I even had the trainer confused as to why we could not get it to work when he was here.