Hello Guest it is May 21, 2019, 11:16:52 PM

Author Topic: The bugs keep coming ??  (Read 2515 times)

0 Members and 1 Guest are viewing this topic.

Offline Sage

*
  •  365 365
    • View Profile
The bugs keep coming ??
« on: October 12, 2013, 07:51:30 AM »
Attention Brian !!
Pretty sure I've discovered another bug in Mach 3. Probably one nobody would ever have noticed. (Then again maybe my code is faulty).

I had a large plate that I needed to chamfer an edge on. I couldn't do it on the lathe so I decided to lay it flat on my rotary table and do it on my mill.
I wrote a simple program to turn the plate and feed down in Z 5thou at a time until I got to .187
I ramped down to each depth by turning 45 degrees while feeding Z down the 5 thou and then leave the Z at depth and continue around to complete the circle.
The code below speaks for itself. It's a very long process but very simple.
About 5 minutes into the process I thought I noticed the rotary table was going faster than when I started out so I adjusted the federate offset to get back to my preferred
2 seconds per revolution of the rotary stepper motor (which translates to 3 minutes per table rev).
The longer the process continued the more I had to slow the process down with the federate offset.
In the end I had the federate offset adjusted for about 1/10 of what it started out at in order to keep the rotary table stepper motor at the same speed.
I couldn't believe what had happened so after the job I ran the process over without a cutter and  let it run without making any adjustments.
Sure enough I started out with a units/min of about 73 on the federate display for units/min.
After 1 hour the units/min had climbed on it's own to more than 600.
The units/rev had also climbed from an initial .04 to .34
I noted that the federate climbs after each part of the code where it performs a Z down feed while rotating 45 degrees. When it goes to the part of the code where it's just rotating around to 360 the speed has increased from what it was last time.

Probably something Brian should look into and be sure it's not a problem in Mach4.

Code is below.
Thanks
Sage

(Uses Z and A axis only - )
G20 (Units: Inches)
G40 G90 G91.1
S1000 (Mill/router, 0.375 in diameter)
T1 M06  G43 H1
S1800 M03

G01 Z0.000 F0.25
Z-.005 A45 (Ramp down 5thou in 45 degrees)
A360 (Do the rest of the circle)
Z-.010 A45
A360
Z-.015 A45
A360
Z-.020 A45
A360
Z-.025 A45
A360
Z-.030 A45
A360
Z-.035 A45
A360
Z-.040 A45
A360
Z-.045 A45
A360
Z-.050 A45
A360
Z-.055 A45
A360
Z-.060 A45
A360
Z-.065 A45
A360
Z-.070 A45
A360
Z-.075 A45
A360
Z-.080 A45
A360
Z-.085 A45
A360
Z-.090 A45
A360
Z-.095 A45
A360
Z-.100 A45
A360
Z-.105 A45
A360
Z-.110 A45
A360
Z-.115 A45
A360
Z-.120 A45
A360
Z-.125 A45
A360
Z-.130 A45
A360
Z-.135 A45
A360
Z-.140 A45
A360
Z-.145 A45
A360
Z-.150 A45
A360
Z-.155 A45
A360
Z-.160 A45
A360
Z-.165 A45
A360
Z-.170 A45
A360
Z-.175 A45
A360
Z-.180 A45
A360
Z-.185 A45
A360
Z-.187 A45
A360 F0.25
Z-.187 A45 (Clean up pass to remove ramp)
A360 F0.25

Z-.15 A45 (Lead out - raise tool while rotating to avoid stop mark)

G00 Z0.01
M05
M05 M30
« Last Edit: October 12, 2013, 07:53:47 AM by Sage »

Offline ger21

*
  • *
  •  6,232 6,232
    • View Profile
    • The CNC Woodworker
Re: The bugs keep coming ??
« Reply #1 on: October 12, 2013, 11:39:47 AM »
You need to enter the radius of your part in the rotation radius box, or uncheck the box in Config Toolpath that adjust the feedrate for rotary axis.
It sounds like Mach3 is compensating the feedrate depending on the radius, if Mach3 knows what the actual radius is.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline Sage

*
  •  365 365
    • View Profile
Re: The bugs keep coming ??
« Reply #2 on: October 12, 2013, 12:16:41 PM »
I'll trust your judgment on this one but I'm not sure why it would be compensating anything. The radius isn't changing. The tool just sits there and the table rotates under it. The only thing changing is the Z axis depth of cut.

I could see if the tool moved toward the center of rotation somewhat then the rotary might want to speed up to adjust the SFM. But that is not the case.

Sage

Offline BR549

*
  •  6,865 6,865
    • View Profile
Re: The bugs keep coming ??
« Reply #3 on: October 12, 2013, 12:50:38 PM »
Mach3 is doing as Ger suggested. The setup for an A axis is normally inline with X and Z 90 degs to X. So that if you lower Z it compensates for the radius difference.

Now if you do not want that option then I believe you can turn it off in config

Just a thought, (;-) TP

Offline Sage

*
  •  365 365
    • View Profile
Re: The bugs keep coming ??
« Reply #4 on: October 12, 2013, 03:33:46 PM »
Ok. I guess that makes some sense.
I'll try fiddling with it to see if I can correct the issue. Now that I'm all done with it -  ;)
And try to remember that for the next time.

Sage

Offline Sage

*
  •  365 365
    • View Profile
Re: The bugs keep coming ??
« Reply #5 on: October 12, 2013, 03:50:47 PM »
Ok. So I had a look in the General Config. The only check box I see that seems related is one labeled "Radius Compensation Off" and it is checked (off). But it's  in the section to do with (I guess) what to do on a system stop, M30 etc. so I'm not sure that's it.

Not sure what to put in the settings screen for "Rotational Diameter". Seems to me anything you put in there might only change how fast it compensates based on what you tell it the diameter is. I don't want it to change at all.

Any ideas what I'm missing?

Sage

Offline BR549

*
  •  6,865 6,865
    • View Profile
Re: The bugs keep coming ??
« Reply #6 on: October 12, 2013, 04:59:10 PM »
On the settings page set A to 0.000 it should turn radius compensation OFF.

OR go to Config/Toolpath then turn OFF use radius for feedrate.

(;-) TP
« Last Edit: October 12, 2013, 05:01:38 PM by BR549 »

Offline Sage

*
  •  365 365
    • View Profile
Re: The bugs keep coming ??
« Reply #7 on: October 12, 2013, 05:56:59 PM »
I would have never looked there for the setting.
Ok. I'll check it out.

Thanks for your help.

Sage