Lathe Radius G7 or Diameter G8 mode

[JJackrabbit]

Hello

I want to use diameter mode instead of radius.

When I go into CAM-> Setup -> I can see 'radial dimension mode'.

But it only shows Radius.

Is it possible to change to diameter?

[kate.raskauskas]

Hi @JJackrabbit,

Thanks for bringing this to our attention! I've logged it with development (ticket CAM-8631).

[Anonymous]

Hi, In a similar subject, when simulating a turning set of operations all seems to work correctly but when I post process with the Mach3 turn post processor file, I get diameter dimensions were it clearly should be radial dimensions resulting in the CNC lathe trying to machine a part twice the size intended. I tried to set Mach 3 to Diameter instead of Radius for the dimension interpretation under the Turning options.  But that did not change anything. Is this a mach 3 post processor file issue or a setting in fusion CAM that I missed? Anyone with an idea how to fix that issue or a work around solution? Thank you.

[GeorgeRoberts]

Hello,

Thanks for posting. You're correct, the Mach 3 post processor is currently set to diameter mode. To change this, open the post processor with a text editor and change this line:

var xFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true, scale:2}); // diameter mode

to this:

var xFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true, scale:1}); // radius mode

hope this helps!

[Anonymous]

Thank you George,

Changing the xFormat like you suggested did the trick.

While we are on the Mach3 post file subject, I found that it generates a G48 S#SpindleSpeed#. I tried to find out what that code do but it is omitted in Mach3 Turn manual. I did find externally from ArtSoft that the G48 is “Tool offset double decrease” command. I am not sure what it does but it seem to be some kind of tool offset compensation. The closest (most similar) command I could find in the manual was "G41/G42
Start nose radius compensation left/right” or “{G43, G49} tool length offset” Should this section of code (see bellow) be modified? At this stage I am not sure if having this G48 in my g-code is an issue or not but I would feel more comfortable to know if it is functional in Mach3 and what are the effect on the part being machined before I try to turn a chunk of steel. Also I find it odd that it has a speed command on the same line “S##”. I am not familiar with the post processing code but It seem that the intension of this code is to set up the spindle speed mode instead (G94 Feed/min mode Vs G95 Feed/rev mode ). Or it may have to do with  Feed and Speed Override M48 and M49 and used a G instead of a M? All this is making my head spin.

I appreciate your help
Thank you again

Post processing code that generate a G48 S##

gSpindleModeModal.reset();
  if (currentSection.getTool().getSpindleMode() == SPINDLE_CONSTANT_SURFACE_SPEED) {
    var maximumSpindleSpeed = (tool.maximumSpindleSpeed > 0) ? Math.min(tool.maximumSpindleSpeed, properties.maximumSpindleSpeed) : properties.maximumSpindleSpeed;
    writeBlock(gFormat.format(48), sOutput.format(maximumSpindleSpeed));
    writeBlock(getCode("CONSTANT_SURFACE_SPEED_ON"), sOutput.format(tool.surfaceSpeed * ((unit == MM) ? 1/1000.0 : 1/12.0)), mSpindle);
  } else {
    writeBlock(getCode(“CONSTANT_SURFACE_SPEED_OFF"), sOutput.format(tool.spindleRPM), mSpindle);
  }

Snip from mach3 turn manual

10.2.1 Feed and Speed Override controls
Mach3 commands which enable (M48) or disable (M49) the feed and speed override
switches. It is useful to be able to override these switches for some machining operations
e.g. threading. The idea is that optimal settings have been included in the program, and the
operator should not change them.

[GeorgeRoberts]

Thank you for your reply. Please could you send me a link to the manual for your machine? I can only find a very old Mach 3 manual...

Many thanks

[Anonymous]

Hi George,

Yes, that is probably the same manual I have found: http://www.machsupport.com/wp-content/uploads/2013/02/Mach3Turn_1.84.pdf
I am not aware of any more recent manual for the mach3 software. The company kind of moved on to their Mach4 version which unfortunately is not compatible with my setup at this time.
The mach3 version I am currently using is:  Mach3Version3.043.022. There is a slightly more recent version: Mach3 R3.043.066 that may solve some specific issues in some special case.

Thank you

[Anonymous]

Hi George,

I did a little more testing and found that the G48 S## gCode command come from the "Use Feed per Revolution" in fusion. When run in Mach 3 it seem to have trouble for the first few pass but then do what it is suppose to. More specifically it will start running very slowly at first then after a few cycles run at the correct speed. So even-though the G48 is not documented it seems to partially work. Not sure what to do to fix the slow start at this point though.

Best,

Yves

[jasengrice]

Question for the original post answer.  Did this ever get fixed in Fusion 360 CAM?  As I still cannot see a way to change from radius mode to diameter mode.  Only one option is there and you can't deselect it or anything.

Thanks,

Jasen

[NewAmericanPublicArt]

Hi George & Kate,

I'm trying to implement a similar solution for the Fanuc Turning post. I changed the line you indicated to:

var xFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true, scale:1}); // radius mode

However, the posted g-code is still reading diameter-based values for all the X coordinates. 

Is there somewhere else I have to make this change in the Fanuc post-processor in order for it to work? Is there a setting I'm missing somewhere in order for this change to take effect? 

Thanks for your help.

[ahmadalsabawi]

Dear George

I used your solution on inventor cam 2022 but it is unfortunately did not work. The software did not response to any scale vale. And the post processor still producing diameter values rather than the radius values for my turning task. I also use mach3. However, I used it on all processors but I always get the same incorrect results.

var xFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true, scale:0}); // radius mode

Reagards

ahmad

[seth.madore]

@ahmadalsabawi you need to set it to scale:1, not scale:0

I just tested this in the most recent Mach3 turning post processor, and changing that line alone was sufficient to correctly produce radius values in the X axis instead of diameter values

[ahmadalsabawi]

I know that zero is not correct. But I used it and used an other values, 1,2,...etc while the x values still the same, which are diameter values.

Question: do I need to have a mach3 post processor in the CAM Tab in the Inventor environment? If so, then whould please send it to me. Can I use some generic post processor ?

thanks

[wexauto]

Has there been any development in this issue? Changing the scaling in the post-processor makes it at least functional, but arc and radius cutting (I,J,K mode) do not work correctly, as well as the DRO and scaling issues. Thank you for your time.