Haas tl lathe using Bobcadcam code

[bobadame]

Please bear with me, I'm a complete noob here. My questions have to do with using Bobcadcam to draw a representation of the part want to make. I understand that I only need to draw half the profile of the part. My first question is: should I draw above or below the Z axis line? The video professor says to draw the half above the Z axis line but then my cutting tools don't make sense as they face opposite of what would be used with a lathe that uses tools coming down from the top. I better just start with that. Thanks in advance.

[Geof]

Don't worry about the tools being on the "wrong" side on the TL1. This machine uses standard programs exactly the same as all the other Haas lathes which have the tools in the correct place.

[bobadame]

So then I should draw above the Z line?

[Geof]

Draw as yo would for a normal CNC lathe.

[bobadame]

Thanks Geof. I guess my problem is that to me this TL is a "normal cnc lathe" and the orientation of the tools and the Bobcad training cd seem to be backwards. I'll get over it.

[Donkey Hotey]

Try to output your code and do whatever it takes to generate positive X values. My guess is that it'll be drawing above centerline, not below it.

[Geof]

Thanks Geof. I guess my problem is that to me this TL is a "normal cnc lathe"....

That is because you are a newcomer to CNC.

CNC lathes nearly always have the tool upside down, at the back with X coming coming down at an angle above the horizontal. That is opposite to a normal manual lathe.

The TL machines are made to operate like a normal manual lathe when they are operated manually. When they are running in CNC mode the controller runs them as a CNC lathe as if the tool was at the back upside down. If you run them in Graphics you will see on the screen the tool path operates this way.

[bobadame]

Thanks guys that seems to be working. The problem now is that the Haas controller gives a warning that the boring tool is too big to fit. I've drawn a 3/8 diameter custom tool in Bobcad and it should show up as a user defined tool but instead it shows up as a dynamiclly drawn tool. In other words, the software is not assigning the geometry that I drew to the name of the tool in the tool list. I'll bang on this some more.

[ggilbert76]

I find that most lathe parts are way easier to program at the control than on a cad can program. I've only used mastercam for mills or to determine points difficult to trig out.

Sent from my Droid using Tapatalk

[Donkey Hotey]

Why exactly are you using BobCad to generate your lathe code? Geof is going to snicker at me for posting this but, lathe parts are generally so simple that I find they're not worth the hassle of using CAM software.

I don't do anything on the mill without using Mastercam but, I still haven't bothered to even learn Mastercam Lathe for our SL-20. The setup seems like more trouble than it's worth.

[bobadame]

That's a good question. It should be simple to do. The job is to create a bore 1.180 ID with a straight length .411 long then at the tangent point, a full spherical radius .590 (half the bore dia.). Simple I suppose for someone who speaks the language. I don't. I spoke with the techs at the local Haas store about this cut and was told that the IPS, Intuitive Programing System. wasn't set up to do this. There is a function called internal turning that gives the option of creating a fillet at the bottom of the bore. I fill in all the blanks with reasonable values and the controller gives me a "non monotonous error". Apparently it only is willing to do monotonous things.

The message is :The path defined by PQ was not monotonic in the x axis. A monotonic path is one which does not change direction starting from the first motion block. Can someone translate this?

[Geof]

The code must have been using G71 a roughing canned cycle.

To use this canned cycle on a bore you start with a drilled hole (of course) and the starting diameter for the boring tool is the drilled hole diameter with the Z position just a bit in front of the part; this position is specified on the line before the line with the G71 command.

The G71 line has a P(number) and a Q(number) which are line numbers in the code below the G71 line; this is the P Q block.

The P Q block contains the code to describe the profile of the bore with the radius at the bottom. This is where monotonous and non-monotonous moves come in. Obviously when you bore a hole with a radius at the bottom the tool moves to a smaller diameter while it is doing the radius; this is a non-monotonous move because the first goes out to a larger diameter then back to a smaller one, the tool reverses its direction of travel on the X axis.

Non-monotonous moves are permitted in a G71 P Q block and this is called Typer II roughing. Type I roughing is monotonic, i.e. the tool does not change direction.

You have to tell the controller you want to do Type II roughing and this is done in the P line of the P Q block by having both an X and Z move; i.e. the tool moves on X to the finished diameter and moves very slightly on Z closer to the part.

You are going to have to puzzle this through a bit by reading the manual as well as my translation here. My manual covers this on page 133 under G71 O.D./I.D. Stock Removal Cycle.

If you post a picture of the part I can maybe write the code for the G71 if you cannot get it sorted out. Incidentally I can only open jpg pictures because i do not have any CAD program on my computer.