Hello Guest it is September 26, 2020, 06:12:59 PM

Author Topic: Real G93 Gcode anyone  (Read 4557 times)

0 Members and 1 Guest are viewing this topic.

Offline Mauri

*
  •  309 309
    • View Profile
Re: Real G93 Gcode anyone
« Reply #10 on: January 30, 2018, 03:17:33 PM »
More attachments,
These are the rest.
You can see in these example that calculating all X/Z/A gives you different results to X/Z and A on separate lines.
Regards,
Mauri.

Offline dude1

*
  •  1,253 1,253
    • View Profile
Re: Real G93 Gcode anyone
« Reply #11 on: January 30, 2018, 03:38:07 PM »
That's from the HSM/Fusion 360 post processor it's java in there extension of .cps

Some machine can handle useing inverse time not all.

It's time of flight so it all tries to move in sink with the rotary motion, if you did not run in sink with the rotary axis the rotary axis moves slow as a wet week or you have to have it's feed rate over 2 times faster than a linear axis to just keep up

Offline Mauri

*
  •  309 309
    • View Profile
Re: Real G93 Gcode anyone
« Reply #12 on: January 30, 2018, 05:46:52 PM »
Dude1,
Thanks for the info.

I manually calcuated this next file.
Attached the same CircleStepTest file, but this time it has both G94 and G93 in the G-Code.

Could anyone try these files as an AIR test as I currently do not have a running 4 Axis for Mach4 and compare the times.
I have included the Simulated cut shape using Predator and all four G93 files run and cut the same shape.
Regards,
Mauri.

Offline dude1

*
  •  1,253 1,253
    • View Profile
Re: Real G93 Gcode anyone
« Reply #13 on: January 30, 2018, 06:27:40 PM »
That shape part does not need inverse time it's 2 moves then one then 2, it's for when you wont to move many axis at the sametime like 3 plus axis, that toolpath I posted is a wrap 4 axis toolpath doing 4 axis moves at onces it makes it more continuous than wrap.

Offline Mauri

*
  •  309 309
    • View Profile
Re: Real G93 Gcode anyone
« Reply #14 on: January 30, 2018, 06:45:19 PM »
Dude1,
Yes I am fully aware of what you are saying, this was a simple example as the forum system cannot receive large 4/5 axis simultaneous G-code.
It does still speed up the cut as it does have variable movement of the A axis.
It also shows the issue, when your axis movements vary (i.e.) when one axis moves a lot more than another as it happens in simultaneous axis machining of statues.
A normal CNC cut would be a spiral cut but would not make a precise shape like the supplied G-Code.

Below are G93 calculations and my take on there results I have calculated.

Full Movement Distance Calculation D= square root of (  dx^2 + dy^2 + dz^2 + a arc_length^2) used in the Gano Technology program.   
Full Movement Distance Calculation D = square root of (dx^2 + dy^2 + dz^2 + a arc_length^2 + b arc_length^2 + c arc_length^2) This would be a 6 axis version   
[where dx is the change in x from the last move, etc.]     
ArcLen =  R * theta   (where R is the current largest Z value) and theta is the change in rotation for that line (converted to radians).  Used in the Gano Technology program.   
G93 Fspeed = G94 Fspeed / D full movement distance.   
This produces an average speed across all Axis.   
   
If calculating Linear and Arc movments seperately then   
D = dx and G93 Fspeed = G94 Feedrate / D (same for Y and X axis)   
D = a arc_length = R (the current largest Z value) x theta (change in rotation for that line canverted to radians) = G94 Feedrate / D (same for B and C axis).
This produces a more accurate result.

For the most accurate Feedrate speed using G93 on all these axis would be if all are calculated individually.   

However if you could mix G93 and G94 in the G-Code, then the only calculation that is required is for the ARC movments as the Linear ones would remain as G94 with its user set feedrate.   
Regards,
Mauri.

Offline RDR

*
  •  22 22
    • View Profile
Re: Real G93 Gcode anyone
« Reply #15 on: January 30, 2018, 07:00:16 PM »
Hi Mauri
I use g93 on our 5 axis Waterjet and it uses it only when the one of the two rotation axis's  are being used but the is also x and y movements all on the same line. I will try to remember to post a code for you to review but it may not help you much but I had to do a lot of digging to help Sigmanest get it to work right.  Also I do know on my machine with mach3 the arc movements we had to divide the feedrate by the arc radius not sure why but that was the way it worked out

Offline Mauri

*
  •  309 309
    • View Profile
Re: Real G93 Gcode anyone
« Reply #16 on: January 30, 2018, 07:17:04 PM »
RDR,
If you are using Mach3 there should be no issue it does not require G93.
For me it can produce accurate speed changes as the Z axis changes the A axis also changes in speed to maintain the correct surface speed.
You must put .0001 in the Rotation Radius under the Settings Tab on your A/B/C if using 4/5/6 axis.
You must also under "ToolPath Configuration" place a TIC in "User Radius for Feedrate".
I have manually calculated the times and compared then to actual times on Mach3 and they are within a decimals second.

As we do not have this available in Mach4 hence the search for an alternate solution.

Regards,
Mauri.

Offline RDR

*
  •  22 22
    • View Profile
Re: Real G93 Gcode anyone
« Reply #17 on: January 30, 2018, 08:02:33 PM »
I wish that would work in my case be it would not the radius that we are cutting are always in one part is always different and our rotation is around the z axis and then throw in a tilt of the head that also is in deg's the g93 is the only way for me

Offline RDR

*
  •  22 22
    • View Profile
Re: Real G93 Gcode anyone
« Reply #18 on: January 31, 2018, 08:43:50 AM »
Attached is two file one has the G93 code that we need to run to make the feed rates right and the other has the normal feed rate.  Like I said this may not help you much since it is not a mill code but you need to have the G93 when you do any rotary movements as you can see in the code  and in the picture that is attached when it is doing the straight line I do not need the G93 but when it comes to the Arc I do

Offline RDR

*
  •  22 22
    • View Profile
Re: Real G93 Gcode anyone
« Reply #19 on: February 02, 2018, 08:12:31 PM »
Did some playing around   But first what cam are you using?  I did some testing on mcam and it looks like it will do a 4th axis feed rate correction and also I posted out a G93 code for you to view see attachment