Hello Guest it is July 17, 2019, 05:16:23 PM

Author Topic: Erratic Feedrate When Cutting Spline Lines  (Read 4265 times)

0 Members and 1 Guest are viewing this topic.

Offline Mauri

*
  •  302 302
    • View Profile
Re: Erratic Feedrate When Cutting Spline Lines
« Reply #10 on: September 25, 2017, 04:04:50 PM »
dq828,
I change all angles 0 to 179.
We do fine engraving in Brass with the finish cuts being with .05mm Radius Tapered Cutter.
This means that we do not know all the angles, as it could basically cover all of them and braking cutter tips is not an option.
Performing a Simulation on the 3D image shows us when we have a good enough CV settings (i.e.) cut follows closely to the original G-Code.
If you know you angles you can modify the CV speed to suit.
Yes you can copy and paste pre edited or programmed settings in your machine.ini over the existing settings and save the file.
You can program in Lua on the Screen yourself a suitable program or modify the exiting CV wizard.

Machine shake:
Reduce F Speed
Reduce CV speed
Fix Machine to prevent kick.
Or use Exact Stop

Regards,
Mauri.

Offline Mauri

*
  •  302 302
    • View Profile
Re: Erratic Feedrate When Cutting Spline Lines
« Reply #11 on: September 25, 2017, 07:13:47 PM »
dq828,
Directional change in CNC machining is a complex physics and mathematical issue.
If you had a machine with magnetic slides then directional movement would not be an issue as the table is held in a magnetic field suspension.
We do not have $500K plus.
As most of us have linear ball slides on Router Tables or V's with Gibbs on Mills we have to contend with a lot more issues.
The better the machine is constructed the faster you will be able to run it.
When a force (Y/Z gantry platform or X/Y table) is being sent in one direction like CV Angle 0 and then you want it to return back you have to stop that table smoothly or come to a complete stop before you change direction back.
The X/Y platform wants to lift off the table making the balls hit the rail guide and shake the machine.
A roller guide connected to the Y gantry and rolling on the bottom edge of the X table on both side would reduce this (hence a better design) or have linear ball rails on the bottom as well the side.
On the Mill the issue on the X and Y are the Gibbs on the V slide, too tight premature wear and tear on the slide and motor or the motor may not be able to move the table at all.
Too loose and the table ants to kick up.
Below are some Physics and Maths on CNC angle movement.
So you need to have the CV on the Angle 0 as this is the maximum shake angle.
Regards,
Mauri.

Offline dq828

*
  •  57 57
    • View Profile
Re: Erratic Feedrate When Cutting Spline Lines
« Reply #12 on: September 26, 2017, 07:27:47 AM »
Thanks for the input, I get the theory even though I dont understand the Maths, it'll be trial and error for me.

Offline Chaoticone

*
  • *
  •  5,524 5,524
  • Precision Chaos
    • View Profile
Re: Erratic Feedrate When Cutting Spline Lines
« Reply #13 on: September 26, 2017, 10:37:11 AM »
Hey Guys,

I have written a wizard that populates the CV table based on the axis you select, their motor tuning (accel and velocity) and a off path by max tolerance that you enter. It will populate the Feed rate for each angle from 0-179 degrees in the CV table that is the max the machine can do and stay within the tolerance you specified. If there is enough interest, hopefully it will be available for testing later today. Let me know if your interested.
;D If you could see the things I have in my head, you would be laughing too. ;D

My guard dog is not what you need to worry about!

Offline Mauri

*
  •  302 302
    • View Profile
Re: Erratic Feedrate When Cutting Spline Lines
« Reply #14 on: September 26, 2017, 03:52:09 PM »
Chaoticone,
Yes that would be of interest to many of us.
Regards,
Mauri.

Offline Chaoticone

*
  • *
  •  5,524 5,524
  • Precision Chaos
    • View Profile
Re: Erratic Feedrate When Cutting Spline Lines
« Reply #15 on: September 26, 2017, 04:56:12 PM »
Here it is guys. For now, it will only be accurate for machines whose machine setup units are set to inch. The tolerance you set is in inches and it populates the CV_Feedrate table in inches per minute. Inches everything.......... everything is inches. Once I feel confident its good to go for inches i will make it so it works for mm as well.

Just download the attachment and place it in your Mach4\Wizards folder. You can then select and run it as any other wizard.

Let me know how it works for you please.
« Last Edit: September 26, 2017, 04:59:12 PM by Chaoticone »
;D If you could see the things I have in my head, you would be laughing too. ;D

My guard dog is not what you need to worry about!

Offline Mauri

*
  •  302 302
    • View Profile
Re: Erratic Feedrate When Cutting Spline Lines
« Reply #16 on: September 26, 2017, 08:54:49 PM »
Chaoticone,
I have made a quick test and have a few questions.
I have included a DOC file that has the data and graph.
Question why does the CV Feedrate exceed the Mach4 Motor settings?
Is angle 0 a straight line?
Why are the Feedrates higher on small angles and zero on the large?
Are the Feedrate the wrong way around?
Regards,
Mauri

Offline Chaoticone

*
  • *
  •  5,524 5,524
  • Precision Chaos
    • View Profile
Re: Erratic Feedrate When Cutting Spline Lines
« Reply #17 on: September 26, 2017, 11:06:52 PM »
Quote
Question why does the CV Feedrate exceed the Mach4 Motor settings?
Feed rate can easily exceed the max of a single axis when more than one axis is feeding. Think blend velocity. To get the blended velocity sum the velocity vectors:
blendVel = sqrt(vX*vX + vY*vY + vZ*vZ). If 2 axis start at 0 and are traveling at 10 units per minute how far has the tool moved in a single minute? Draw a 10 unit line in X and one in Y then measure destination to destination. You will see that while neither axis moved over 10 units a minute the tool would have traveled quite a bit further.

Yup, a line of 0 degrees is a straight line.

Why do you have to slow down in your car to make a 90 degree turn? I blame it on the *^&^ that wrote the laws of physics but until someone does better I guess I will have to abide by those laws. Think about it.... your going down the road at 100 miles and hour or 5 miles an hour or just walking, or riding a bike..... any kind of motion. How much do you have to slow down to change your path by 1 degree Vs. changing it by 90 degrees Vs changing it by 179 degrees (1 degree off from being the exact opposite direction). This is why the table ends at 179 degrees. No way to go in exact opposite without first stopping. What happens if you don't slow down? You go off path, possibly by a lot as in through the ditch and in the corn field lot.

Nope, smaller angles can be ran much faster than larger angels while each maintain a set tolerance to the requested path.

How do your tool paths measure up using the wizard?
;D If you could see the things I have in my head, you would be laughing too. ;D

My guard dog is not what you need to worry about!

Offline dq828

*
  •  57 57
    • View Profile
Re: Erratic Feedrate When Cutting Spline Lines
« Reply #18 on: September 27, 2017, 05:31:56 AM »
I'm looking forward to the mm version :)

Thanks, you have answered a lot of my questions, but I have more :) always more!

If you select Constant Velocity in the Mach Configeration Menu and you dont go to the Wizard or adjust any settings in the .ini file I assume the machine behaves just like it would if Exact Stop was set.

Previously I had selected Constant Velocity and then later found out about the Wizard, when I went into the Wizard for the first time all angles were 0 and the CV Feedrate On/Off button was set to Off, even though I had selected Constant Velocity in the Configeration Menu. So the way I see it is selecting Constant Velocity in the Configeration menu actually does nothing unless you change the settings in the Wizard, is that right?

My plan was to set 0 degrees  to the full feed rate I generally use and then gradually decrease the feedrates and probably have 0 in a lot of the tighter angles

Offline Mauri

*
  •  302 302
    • View Profile
Re: Erratic Feedrate When Cutting Spline Lines
« Reply #19 on: September 27, 2017, 07:37:44 AM »
Chaoticone,
Your wizard Simulated with the Road Runner runs very well in inches.
I too use Metric mm and it is a bit time consuming to set up and test in metric, so I look forward to seeing it in Metric version.
When I engrave in Brass with a .05mm Radius Tapered cutter I do not want to exceed my G-Code settings of 400mm/sec this way my cutter can do multiple 12 hours cuts with no cutter damage.
So in your Wizard can you add a Maximum Velocity speed so when it writes the data to machine.ini it will replace all the higher numbers with this G-Code maximum?
It also appears from your explanation that the Angle is measured from the Back plane and not the Front.
So the 179 degree is actually a sharp point movement and a 1 degree is 1 degree less then a straight line.
On our 3D medallion which we carved recently I used 100mm/min on all angles on all 3 axis with the normal straight cut running at 400mm/min and they came out reasonably well viewed under a microscope.
Your method would reduce the cutting time and still obtain a good result and on top of that be able to increase accuracy with your tolerance option.
Looking forward to seeing the update in Metric with hopefully the G-Code Maximum Velocity inclusion else cutters will be broken.
Regards,
Mauri.