Corner rounding

More
29 Apr 2018 17:18 #109809 by smplc
Corner rounding was created by smplc
Semi-finish turning an outer diameter profile with a right hand tool, .0312 tool nose radius (TNR), tool nose orientation (TNO) 2 and enabling cutter compensation (G42). No rough turning outer diameter at this time due to example and wire frame. Program coordinate Z-.5000, DRO, tool nose compensation only Z-.5312 which, isn't far enough and should be Z-.5396 before, executing descending 210 (30) degree angle. When executing 210 angle a small radius is left at .5000 dimension. End point of small radius isn't seen on DRO, Step and simultaneous into 210 degree angle. Did the program not read ahead for next line, is a droop, reenable cutter compensation or no correspondance with TNO of particular tool path? After executing 210 is Z-.7896 which, is accurate cutter compensation and -.7500 dimesion. Suspected is that the 210 is mostly an accurate angular plane if correct cutter compensation at -.7500 dimension. Simulation showed that rest of the profile tool nose of cutter compensation accurate.

Attempted to use a TNO 6 and TNR .0312 as demo and if Z-.5000 would compensate accurately. And attempted to use TNO 2 and TNR .0156 as demo and if Z-.5000 would compensate accurately. Either didn't. The rest of profile remained cutter compensation accurate.

Tried G61, G61.1 and G64 P.0005. It didn't correct the unexpected corner rounding. Is a feature in AXIS lathe control panel to enable and disable if corner rounding?

Please Log in or Create an account to join the conversation.

More
02 May 2018 22:24 #110061 by andypugh
Replied by andypugh on topic Corner rounding
I don't actually understand the question. Can you say what you expected and what actually happened?

What did the workpiece look like? Be aware that the Axis preview shows the tool control-point path, not the work.

Are you sure that your tool orientation is correct (a historical accident means that tool orientations in LinuxCNC do not match Fanuc. It is hard to change now)

Please Log in or Create an account to join the conversation.

More
03 May 2018 04:06 - 03 May 2018 04:45 #110085 by smplc
Replied by smplc on topic Corner rounding
Yes. 210 degree angle must intersect centerline of .0312 tool nose radius tangent before executing it's path. Therefore Z-.5000 requires an additional -.0396 to intersect that angular plane. If not the tool nose radius undercuts the angle.

I haven't cut a physical workpiece of this particular dimension with lathe yet. I opened my mous.ngc program with sim.axis lathe. My CNC micro lathe isn't configured with 7i92.ini and .hal hostmot2 file yet. .ini might require [LATHE] = TRUE and LATHE = 1 to enable lathe mode.

I know from industrial experience operating CNC lathes, single block and GE Fanuc and Okuma controls that tool nose compensation offsets itself as described. Nonetheless centerline of tool nose radius is expected tangent of angular plane before executing it's path. It might vary and some CNC controls could compensate X and Z tool nose radius simultaneous and tangent of angular plane but seems seldom while already on longitudinal path. If X and Z compensation X might leave a faint witness mark, a shallow groove and slightly undercuting.

Aware that LinuxCNC AXIS lathe control could compensate slightly differently than an industrial control but it seems comparable. Except that one plot Z-.5000 didn't offset itself far enough. Again could be an X and Z simultaneous offset but it appears a magnifide radius is left and might be an undercut. It's such a small amount with a .0312 tool nose radius and Z-.7896 tangent that it might not matter. Such if a .0625 tool nose radius then it's could be a lot more error if not compensating beyond centerline of Z-.5000.

Not sure if it's LinuxCNC tool nose orientation. It appears +X is bottom half of front view and wire frame. Then tool nose orientation would be 2 (P2). Not sure if cutting troughs with compensation is part of P2, Python interpreter and that Z-.5000 plot. Known that some industrial CNC lathes won't compensate accurately unless per system, tool geometry, orientation and tool path. Reminder leading edges of tool nose radius is touched-off and it's where compensation occurs rather than centerline.
Last edit: 03 May 2018 04:45 by smplc.

Please Log in or Create an account to join the conversation.

More
03 May 2018 10:25 #110104 by smplc
Replied by smplc on topic Corner rounding
Travel expected diagonal and simultaneous to nearest point if X and Z compensation from Z-.5000. That tool nose radius would undercut an angular corner before executing 210 degree angle. Could then what appeared corner rounding be an angle due to computer screen graphic or resolution? The corner does look as if it has an arc to it.

Usually if diagonal X and Z compensation it's lead-in depending on geometry and coordinate of tool before executing tool path.

Mismatch of a continuous profile rare unless backlash or variance of indexable carbide insert and tool nose radius due to mold or honing.

Please Log in or Create an account to join the conversation.

More
03 May 2018 11:46 #110105 by andypugh
Replied by andypugh on topic Corner rounding
I am afraid that I am not fully understanding what you are saying but I will say that LinuxCNC uses the same offsetting for lathe and mill, so on a lathe it assumes that the tool is a circle of the specified radius, So it does follow a true tangent to the path, but does not take in to account the tool front angle and back angle.

linuxcnc.org/docs/2.7/html/lathe/lathe-u...e_tool_orientation_a

Shows the relationship between the control point and the tool centre. These orientation numbers are shown for a front-toolpost lathe and are not the same as some other controls.

The cross will be on the line for plain X and Z moves. The path falls between the tool nose and the cross for angled and curved moves (as it should).

You can see this by watching the preview. Run the code once with compensation on and radius = 0 and then again with a big radius. The path will be inside the first path on the preview but you will see the radius of the tool is tangent to the first path on the second run.

Please Log in or Create an account to join the conversation.

More
03 May 2018 12:36 #110108 by smplc
Replied by smplc on topic Corner rounding
Understood. Resemblance. My desription alike a component of mechanical drafting or engineering.

Please Log in or Create an account to join the conversation.

More
03 May 2018 16:37 - 03 May 2018 16:41 #110126 by smplc
Replied by smplc on topic Corner rounding
.6000 OD
.9000 OD
.5000 x 14.036 degrees

Control point equivalent to tool nose radius tangent on 14.036 degree angle at X.6000 Z.1; Z-.0267 lead-in and Digital Read Out. Next plot at X.8974 Z-.5223. Last plot would of been expected nearer X.9000 Z-.5267.

My calculated plots are X.6000 Z.1; Z-.0271 and X.9000 Z-5271. They could be about a couple minutes off.

Anyhow, it still appears as if corner rounding with control point. Is it automatic corner rounding? Automatic corner rounding is complimentary with Mach4 earlier builds and can be enabled or disabled at control panel Motion Mode or G61. Such any auto corner rounding with LinuxCNC preference is to disable. Any auto corner rounding and if a bigger tool nose radius corner rounding might not get any bigger if not miscompensating.

Foregoing lead-in on tangent angle of workpiece to compare compensation. Generally my angular lead-in coordinates are X_ Z0.020 depending on tool nose radius and not to leave a witness mark before profile.
Last edit: 03 May 2018 16:41 by smplc.

Please Log in or Create an account to join the conversation.

More
03 May 2018 17:32 #110130 by andypugh
Replied by andypugh on topic Corner rounding
I don't think that there is necessarily a problem here.
The Axis preview shows the motion of the control point, not the shape of the material remaining.

If you make one pass with zero tool radius then the control point should trace the material and leave a line on the display corresponding to the material outline.
Then change the tool radius and run again without clearing the preview.
I think you will find that the nose of the tool runs tangent to the first line.

Please Log in or Create an account to join the conversation.

More
03 May 2018 18:23 #110136 by smplc
Replied by smplc on topic Corner rounding
Understood.

A tool nose radius is useful to increase feed rates, to resist wear and improve surface finish. Convenient about tool compensation is that virtually any tool nose radius could offset itself within boundary of workpiece geometry.

I can probably work around the round corner meantime. I'll program a specific size radius on corner outer diameter taper mid-way length and monitor accuracy. Maybe programming a miniature radius could correct it. Or, disable tool compensation (G42) and calculate tool nose radius in program. This could make it complicating but cutter is expected where to be and could prevent lead-in and lead-out errors.

Please Log in or Create an account to join the conversation.

More
03 May 2018 18:34 #110137 by andypugh
Replied by andypugh on topic Corner rounding
Yes, I know that tool radius is useful. I am not suggesting using a zero-radius tool.

But you seem to be worrying about the display on the screen, not the shape of the work.

If you set the tool radius to zero then the display on the screen will be the shape of the work.
If you then set the tool radius to suit the real tool then you should see that the tool follows, accurately, the shape of the work.

And you will probably find that there is not any corner rounding. What you see is what it takes to make a sharp corner with a radiused tool.

Please Log in or Create an account to join the conversation.

Moderators: piasdom
Time to create page: 0.105 seconds
Powered by Kunena Forum