What's new
What's new

Lathe program eliminating small fillet

How? I would imagine that machine comp would be like it is on the mill, no? Just offsets a tool location path by an input value defining the tool?

Just like on a mill.
If you're asking the control to make a smaller inside radius than the radius of the tool itself, then it will alarm.
Of course, that requires the input of the proper radius in the offset page of the tool.
 
Just like on a mill.
If you're asking the control to make a smaller inside radius than the radius of the tool itself, then it will alarm.
Of course, that requires the input of the proper radius in the offset page of the tool.
That's what I thought, yeah. Wouldn't have helped me here, because I told CAMWorks that I was using a tool with radius 0.008 anyway. The tool I put in the machine was incorrect, but I told everything involved that I put the right tool in there.
 
Wouldn't have helped me here,

No, perhaps not in your current situation, but once you get used to comping on the control vs. in CAM, a good deal of this garbage would be avoided.
I know that comment flies in the face of the majority of the members here, but f@ck it, I am standing by my preference of comping on the control for full radius (Lathe) or full diameter (Mill), and never ever to wear, most certainly NEVER!!! use CAM to adjust for size.
 
This crashes the tool. I'm moving toward the spindle and away from center where operator side is +X and left of the bed is -Z using a right handed tool. Seeing as the movement is physically clockwise, I programmed properly using a G02.
It makes no difference to the Circular Interpolation commands used whether the Cutting Tools are at the front of the machine (Cutting Tools are between the Operator and the Workpiece), or at the rear of the machine (Workpiece is between the Operator and the Cutting Tools), provided the X Plus Direction in both instances is away from the Centre Line.

1. A Right Hand OD Tool mounted at the rear of the machine, cutting towards the Chuck that is at the Left of the machine, will be upside down, with the Insert facing down.

2. A Right Hand OD Tool mounted at the front of the machine, cutting towards the Chuck that is at the Left of the machine, will be upside up, with the Insert facing up.

It's as if the whole of the X Axis Slide was rotated about the Centre Line of the machine, thus placing the downward facing insert when the tool was mounted at the rear of the machine, to be facing up when mounted at the front of the machine and bringing the X Plus Direction with it.

So, when the X Plus Direction is away from the machine's Centre Line, with the Tool Mounted at the front of the machine, the Tool Path direction of a Circular Interpolation move, MUST be viewed as if laying on the floor looking up. Accordingly, when viewed from the correct vantage point (from underneath), the movement is physically Counterclockwise. What I have written is a "Chiseled in Rock" convention, and unless there is something wrong with your machine (parameters, whatever), you have programmed it incorrectly with G02.

Regards,

Bill
 
Yes, in your example G2 does not comply with immutable programming convention, which was developed from mathematical norms . Something is funny somewhere.

There are three principle planes, XY(G17), YZ(G19), and ZX(G18). You should say ZX, not XZ. In your example you are machining in the ZX plane.

The Features in Question.PNG
Z+ to the right, X+ down

Your above statement doesn't match your drawing, and it should. Look at your drawing and you will see the axis icon shows x+ pointing up. Your toolpath is drawn on the x minus side, but x numbers in your program example are positive. The toolpath should be along the top surface of the part so the x output is positive, as your machine wants. Then the interpolation in question is G3 rather than G2. That may not match what you see as you stand in front of your machine, but it is correct. Why your machine wants G2 rather than G3 remains a mystery. Maybe your CAM is set up wrong or your post processor or your machine. It might be worthwhile to note when you stand in front of an engine lathe you are looking down on the back, or negative side of the ZX plane.

Often the CAM toolpath does not mimic what you see when standing in front of the machine. Here is a foolproof way to determine correct interpolation sense.

Consider the principle plane in which you are working, ZX. Look at the first axis designator, Z. Travel from the POSITIVE Z axis to the POSITIVE X axis. If you have traveled CCW, you are looking on the positive, or front side of the ZX plane. Now G2, G3, G41, G42 appear as expected, i.e. G2 is CW, G3 is CCW, G41 is tool left, and G42 is tool right. The tool type diagram also appears as expected.

Conversely if you have traveled CW you are looking at the negative, or back side of the ZX principal plane. G2, G3, G41, G42 will now appear backwards, and tool type is backwards.

This convention works for XY and YZ planes as well. CCW travel from the first axis to the second axis confirms the positive side of the plane and everything is as it seems. Again CW travel and you are on the back side and everything seems backwards.

This method eliminates all other questions. No worries about where you are standing, what hand the tool is, comparison to another machine, or if the chuck is on the right or left. It also works for any type of machine tool, not just lathes. When sketching the toolpath, I find it helpful to align the first axis horizontally positive to the right and the second axis positive pointing up. No matter how the machine actually configured. Sometimes this will have you machining on the negative side of one or both axes, but this should mimic what is actually happening on your machine.
 
This method eliminates all other questions. No worries about where you are standing, what hand the tool is, comparison to another machine, or if the chuck is on the right or left. It also works for any type of machine tool, not just lathes. When sketching the toolpath, I find it helpful to align the first axis horizontally positive to the right and the second axis positive pointing up. No matter how the machine actually configured. Sometimes this will have you machining on the negative side of one or both axes, but this should mimic what is actually happening on your machine.
That only works if in the case of a Lathe where the Tool is at the front of the machine and positive X is towards the operator. In the case of a Lathe where the Tool is at the Front of the machine and Negative X is towards the operator, a Convex, OD Radius with the tool moving along the Z axis from Right to Left, will be G02 instead of G03.

Take for examples machines like Mazak M Series Lathes, M4 - M5 etc. where OD tools are at the front of the machine, with +X towards the operator and on the same solid slideway, a Rear Turret is set up with ID Tools, with -X away from the operator and Centre Line. When machining a Convex ID Radius with boring bar in the rear turret, the Circular Interpolation Command will be G03 when the tool is moving along the Z axis from Right to Left. With a typical CNC Lathe where the Tool Turret is at the rear of the machine and +X away from the operator and Centre Line, a Convex ID Radius with the Tool moving along the Z axis from Right to Left, the Circular Interpolation Command would be G02.

Regards,

Bill
 
That only works if in the case of a Lathe where the Tool is at the front of the machine and positive X is towards the operator. In the case of a Lathe where the Tool is at the Front of the machine and Negative X is towards the operator, a Convex, OD Radius with the tool moving along the Z axis from Right to Left, will be G02 instead of G03.

Take for examples machines like Mazak M Series Lathes, M4 - M5 etc. where OD tools are at the front of the machine, with +X towards the operator and on the same solid slideway, a Rear Turret is set up with ID Tools, with -X away from the operator and Centre Line. When machining a Convex ID Radius with boring bar in the rear turret, the Circular Interpolation Command will be G03 when the tool is moving along the Z axis from Right to Left. With a typical CNC Lathe where the Tool Turret is at the rear of the machine and +X away from the operator and Centre Line, a Convex ID Radius with the Tool moving along the Z axis from Right to Left, the Circular Interpolation Command would be G02.

Regards,

Bill
Bill in both your examples, is any machining being done in the x minus direction, or are all programmed x values positive. Just trying to visualize your scenarios.

Greg
 
Bill in both your examples, is any machining being done in the x minus direction, or are all programmed x values positive. Just trying to visualize your scenarios.
In the case of the Mazak M Series, the OD and ID tools are on opposite sides of Centre Line; OD tools operating in +X at the front of the machine, ID tools operating in -X at the rear of the machine. The Tools operating in the -X are programmed for Circular Interpolation, opposite to convention.

Visulaise the two turrets of the M Series Mazak attached to the one solid X Axis, the OD tools at the Front of the machine and +X towards the operator. In this case, an OD, Convex Radius, with the Tool moving along the Z Axis Right to Left, the circular move would be programmed G03. The ID Tools on the same Slideway, on the -X side of Centre Line, would be following the same Tool Path direction as the ID Tool at the Front of the machine. Therefore, to cut a Convex Radius in the bore with the Tool moving along the Z Axis Right to Left, must also be G03. With a machine where the ID Tool is mounted at the rear of the machine and +X is away from the Centre Line towards the rear of the machine, an ID, Convex Radius, with the tool moving along the Z Axis Right to Left, would be programmed with G02.

It's as I stated in an earlier Post, when the Tools are at the Front of the Machine and +X is away from the Centre Line towards the operator, it's the same as if the X Axis Slide was rotated about the Centre Line of the Machine, with the RH tool being Insert Facing up and +X now at the front of the machine. G03 is still CCW, but viewed from below, looking up.

Regards,

Bill
 
I have 3 Fanuc's, and one Mits with a turret in the front (some also have another turret in the back as well) and they all program as if they were rear turrets.

If Milltronics botched this up, that's just another reason to avoid.


--------------------

Think Snow Eh!
Ox
 
Look at your drawing and you will see the axis icon shows x+ pointing up. Your toolpath is drawn on the x minus side, but x numbers in your program example are positive.
Correct. That's why I mentioned that CAMWorks wants it programmed this way, but the machine wants the post to invert everything so I wrote it to do so. I would prefer everything to match up, but it doesn't. It's one of the reasons I don't like working with CAMWorks and I'm going to swap to something else the moment I can manage it.
Then the interpolation in question is G3 rather than G2.
I agree that in that situation I would be using G03 and not G02.
That only works if in the case of a Lathe where the Tool is at the front of the machine and positive X is towards the operator. In the case of a Lathe where the Tool is at the Front of the machine and Negative X is towards the operator, a Convex, OD Radius with the tool moving along the Z axis from Right to Left, will be G02 instead of G03.
OK so maybe when I wrote the post processor I took what CAMWorks was trying to do and flipped everything so it came out right. CAMWorks is programming things like this, and then my post is having the controller match orientation but reverse the X axis.


On a very basic level, all I know is that the machine moves how I ask it to 😆
 
On a very basic level, all I know is that the machine moves how I ask it to
The vast majority of CNC Lathes follow the convention. If you work for yourself and purchase more lathes, strong chance you will be coping with the unconventional and conventional. If you work for someone and at some point, you change employment, it's likely you will have to relearn the way you program.

It's as Ox suggests: "If Milltronics botched this up, that's just another reason to avoid."

The following pictures, Copied and Pasted from a Fanuc Manual, illustrates the flipping of the X Axis about the Centre Line. In each case, +X and +Z are in the direction of the Axes arrows. Everything, including TNR Comp follows the convention of the direction of +X. When determining the direction of Compensation for the Tool and +X at the Front of the machine, at first glance you would have to say that the Comp for a RH OD Tool would have to be to the Left and therefore, G41. However, the same as when determining the correct command to use for Circular Interpolation, you view it from below, looking up.

Regards,

Bill
Typical Configuration of a machine with Tools and +X at the Rear of the machine.
+X to Rear.JPG
Typical Configuration of a machine with Tools and +X at the Front of the machine
+X to Front.JPG
 
Last edited:
OK so maybe when I wrote the post processor I took what CAMWorks was trying to do and flipped everything so it came out right. CAMWorks is programming things like this, and then my post is having the controller match orientation but reverse the X axis.
That's just added more confusion. Where is +X on your machine, towards the Front or Back? There is Zero reason why CAMWorks can't match the characteristics of your control. If +X and the Tools at the Front of the Machine, you simply draw the component and Post Process the Tool Path the same as you would a machine that has +X and the Tools at the Rear of the Machine. If -X and the Tools are on the same side of Centre Line, you simply draw and run the Tool Path on the negative side of Centre in CAMWorks.
 
I seen a Milltronics lathe at The Tool Show several years ago, and I was waiting for it to break in half just sitt'n there.
I can say that it did NOT put me in mind of my Monarch!


--------------------

Think Snow Eh!
Ox
 
In the case of the Mazak M Series, the OD and ID tools are on opposite sides of Centre Line; OD tools operating in +X at the front of the machine, ID tools operating in -X at the rear of the machine. The Tools operating in the -X are programmed for Circular Interpolation, opposite to convention.

Visulaise the two turrets of the M Series Mazak attached to the one solid X Axis, the OD tools at the Front of the machine and +X towards the operator. In this case, an OD, Convex Radius, with the Tool moving along the Z Axis Right to Left, the circular move would be programmed G03. The ID Tools on the same Slideway, on the -X side of Centre Line, would be following the same Tool Path direction as the ID Tool at the Front of the machine. Therefore, to cut a Convex Radius in the bore with the Tool moving along the Z Axis Right to Left, must also be G03. With a machine where the ID Tool is mounted at the rear of the machine and +X is away from the Centre Line towards the rear of the machine, an ID, Convex Radius, with the tool moving along the Z Axis Right to Left, would be programmed with G02.

It's as I stated in an earlier Post, when the Tools are at the Front of the Machine and +X is away from the Centre Line towards the operator, it's the same as if the X Axis Slide was rotated about the Centre Line of the Machine, with the RH tool being Insert Facing up and +X now at the front of the machine. G03 is still CCW, but viewed from below, looking up.

Regards, Bill

Bill, I believe this sketch is what you are describing.

20221227_062736.jpg

If the sketch is correct, then then everything is as I described. The sketch is looking at the back side (or bottom if you prefer) of the ZX plane, as confirmed by traveling from Z+ to X+ in a clockwise direction. Everything is backwards since we are looking at the back side of the plane. If you flip the paper about the horizontal axis (and the paper was see-through), Then Z+ to X+ is CCW and everything is right with the world.

You are saying the same thing when you say:

"It's as I stated in an earlier Post, when the Tools are at the Front of the Machine and +X is away from the Centre Line towards the operator, it's the same as if the X Axis Slide was rotated about the Centre Line of the Machine, with the RH tool being Insert Facing up and +X now at the front of the machine. G03 is still CCW, but viewed from below, looking up."

So if you arrange your thinking so Z+ to X+ is CCW, this machine follows the convention.

After struggling with the "this machine is backwards" deal for a while, this way of visualizing things is easier and seems less confusing, at least for me.

Another "this machine is backwards" deal happens when the machine table moves to position while the cutting tool is stationary. Maybe the mill table moves X- to position the tool to X+. I've heard guys say, "But X is backwards on this machine." But not if you always think about the tool moving, whether it does or not. The coordinate system should always be considered stationary with a moving tool.

Greg
 
Bill, I believe this sketch is what you are describing.

View attachment 382547

If the sketch is correct, then then everything is as I described. The sketch is looking at the back side (or bottom if you prefer) of the ZX plane, as confirmed by traveling from Z+ to X+ in a clockwise direction. Everything is backwards since we are looking at the back side of the plane. If you flip the paper about the horizontal axis (and the paper was see-through), Then Z+ to X+ is CCW and everything is right with the world.

You are saying the same thing when you say:

"It's as I stated in an earlier Post, when the Tools are at the Front of the Machine and +X is away from the Centre Line towards the operator, it's the same as if the X Axis Slide was rotated about the Centre Line of the Machine, with the RH tool being Insert Facing up and +X now at the front of the machine. G03 is still CCW, but viewed from below, looking up."

So if you arrange your thinking so Z+ to X+ is CCW, this machine follows the convention.

After struggling with the "this machine is backwards" deal for a while, this way of visualizing things is easier and seems less confusing, at least for me.

Another "this machine is backwards" deal happens when the machine table moves to position while the cutting tool is stationary. Maybe the mill table moves X- to position the tool to X+. I've heard guys say, "But X is backwards on this machine." But not if you always think about the tool moving, whether it does or not. The coordinate system should always be considered stationary with a moving tool.

Greg
The confusion for many, when programming a lathe that has the Tool Turret and +X at the front of the machine, is that they visualize the Circular Tool Path from their viewpoint standing in front of the machine and see an OD, Convex Radius, with the tool moving from right to left, as being CW. As G02 is defined as Circular Interpolation Clockwise, they mistakenly specify
G02 in the program.

Some of my clients that have such machines and as the programming manual for the machine specifies G02/G03 as CW and CCW respectively, won't accept that the manual is correct until I explain it by having them visualize the Turret and +X at the rear of the machine being rotated about the Centre Line of the machine, including the operator, who would now be at the rear of the machine, standing on their head.

Regards,

Bill
 








 
Back
Top