# What causes jittery movements when running at faster IPM



## Ryan360 (Jun 22, 2015)

So when im cutting at like 60-80 ipm (doing a radius, or something other then a straight line, it gets very jittery and the whole machine tends to vibrate, which is kinda obnoxious and annoying lol. Any way whats the best way to eliminate that? Im guessing its the stepper drivers, seeing how i didn't spend a whole lot on them. This is the kit i got ( stepper motor kit ) 

I use cut2d to generate most of my gcode, but every now and then mastercam from a friend. And use mach3 as the controller.

Any input would be appreciated!


----------



## Stick486 (Jan 4, 2013)

slow down..use sharp bit...
smaller bites...
all or all of the above...


----------



## Ryan360 (Jun 22, 2015)

Wheres the fun in slowing down?  
I dont think they are the problem. Its more it acts like it cant read the gcode fast enough. 
Like it pauses between each line of code and causes a stop for a split second.


----------



## Stick486 (Jan 4, 2013)

Ryan360 said:


> Wheres the fun in slowing down?
> I dont think they are the problem. Its more it acts like it cant read the gcode fast enough.
> Like it pauses between each line of code and causes a stop for a split second.


look to the mechanical drives and not the software...


----------



## 4DThinker (Feb 16, 2014)

Going too fast doesn't let the bit remove the chips it cut fast enough, leaving them there to bump over on the next revolution. The best speed for any bit depends on depth of pass, number of flutes on the bit, full pass or stepover pass, RPM of the router, and material being cut. If you hear the router slow down or struggle, notice excessive vibration, or see smoke coming from the bit, then your speed is wrong. With smoke you are moving too slow. The heat generated isn't being removed with the chips that fly away. 

4D


----------



## Scottart (Jan 8, 2015)

I had a similar problem at over 200 IPM on my big machine, but only when traveling in the X direction.. To Sticks point, the issue was a slightly loose track wheel that held the gantry down on the rail system. so every vector change, which generated a force surge was visible to the eye, but only when trying to go in the X direction.

I discovered this by rotating my tool paths 90 degrees. originally my carvings had long X runs, when I switched to long Y runs the jitters were gone.. Like Stick said, look to the mechanics, not the electronics.


----------



## MEBCWD (Jan 14, 2012)

One thing you need to consider is the number of nodes in the toolpath. A lot of times when fitting vectors to a picture or offsetting vectors from other vectors there will be hundreds or thousands of nodes created around a curve. Check your design file to see if this might be the problem.

Gcode is written written so it runs from one node to the next node then the next node...... If gcode is generated with these vectors with too many nodes the gcode will be create a large file that causes the machine to start and stop start and stop start and stop all the way around the curve. If you use a curve fit function on the vector before generating gcode it will greatly cut down the number of nodes in the vector thereby limiting the number of times the machine stops and continues with the next line of code while cutting around a curve. If a curve only has a starting node and an ending node the curve will be cut with one smooth cut from beginning to end. This also reduces the time it takes for the machine to cut around a curve and reduces the overall time it takes to finish cutting your project.


----------



## MEBCWD (Jan 14, 2012)

Here is an example:

You have a vector in your file and then offset that vector by 0.25. 

The original vector contains 8 nodes.

The offset vector contains .... I don't want to count them .... you can if you want to know how many nodes the vector contains.

The curve fit optimized vector contains 9 nods.


----------



## Scottart (Jan 8, 2015)

MEBCWD said:


> One thing you need to consider is the number of nodes in the toolpath. A lot of times when fitting vectors to a picture or offsetting vectors from other vectors there will be hundreds or thousands of nodes created around a curve. Check your design file to see if this might be the problem.
> 
> Gcode is written written so it runs from one node to the next node then the next node...... If gcode is generated with these vectors with too many nodes the gcode will be create a large file that causes the machine to start and stop start and stop start and stop all the way around the curve. If you use a curve fit function on the vector before generating gcode it will greatly cut down the number of nodes in the vector thereby limiting the number of times the machine stops and continues with the next line of code while cutting around a curve. If a curve only has a starting node and an ending node the curve will be cut with one smooth cut from beginning to end. This also reduces the time it takes for the machine to cut around a curve and reduces the overall time it takes to finish cutting your project.


Ok, that sounds fascinating. when I look at my curves they have tons of nodes.. how do you get rid of those?


----------



## 4DThinker (Feb 16, 2014)

Nodes being the problem would show up no matter what feed speed is used. If they ARE the problem then check the post processor being used for a G64P*** command in the header of your g-code files. If missing or it has no value after the P then add/change it to G64P.005 or something close. This tells the CNC to use best speed from node to node but stay within .005" of them. A large value or no value will have the CNC coming to a stop at each node before processing to the next one. Mike's example above with short line segments making up the curves is typical of drawings I see that are imported from other CAD programs.

4D


----------



## Ryan360 (Jun 22, 2015)

Thanks all for the input, im pretty sure my feeds and speed are right. 
It might have alittle to do with what mike said about the nodes, and the way the gcode is generated. I usually dont notice this problem unless im trying to carve text really fast, or doing a bunch of direction changes really fast. Can the stepper drivers have affect on this? If so what kind and brand should i look into?


----------



## MEBCWD (Jan 14, 2012)

In Vectric VCarve and Aspire there is a tool to fit curves to selected vectors.

You select the vectors then click on the tool icon. It opens a menu for you to enter values depending on how close you want to fit nodes to the curves. You can preview the selected values before accepting the results. You can create new vectors and delete the old one or keep both of them just in case you find the selection won't work. You can select one or more vectors and it will optimize all of them.

I'm sure other programs would have a similar tool.


----------



## Scottart (Jan 8, 2015)

you guys understand this stuff at the atomic level... fascinating... i just hit the "go fast button' than sand it more..

great input.. i am going to have a beer and try to grasp what is being said.. after I hit the Go fast button again...


----------



## Ryan360 (Jun 22, 2015)

MEBCWD said:


> In Vectric VCarve and Aspire there is a tool to fit curves to selected vectors.
> 
> You select the vectors then click on the tool icon. It opens a menu for you to enter values depending on how close you want to fit nodes to the curves. You can preview the selected values before accepting the results. You can create new vectors and delete the old one or keep both of them just in case you find the selection won't work. You can select one or more vectors and it will optimize all of them.
> 
> I'm sure other programs would have a similar tool.




Thanks for your time put into helping me with this, i will have to give what your saying a try!


----------



## honesttjohn (Feb 17, 2015)

Good info, Mike!!

HJ


----------



## MEBCWD (Jan 14, 2012)

When I first started using the curve fit tool I was surprised at how much time I did save cutting some of my files. I just offset vectors and never looked at them. One day I was editing a file and went to node edit some vectors and discovered I had a lot more nodes than I thought there would be. 

As an example, using 2 lines 24" long and one has 2 nodes, a start point and an end point and the other line has 480 nodes equally spaced at 0.05" apart, the tollpath feed rate is set at 100 IPM.

The line with 2 points will cut a lot faster because it will start cutting at the first point, reach the full feed rate of 100 IPM quickly and cut to the end point at full speed, then load the next line of code.
The line with 480 nodes will start cutting at the first node, cut to the second node 0.05" away, stop, load the next line of code and cut 0.05" to the next node, stop load the next line of code .... to the end point and never reach anywhere near 100 IPM while cutting the same length of line.

The gcode file is also much larger for the second line, he first line has one line of code to execute, the second line has 480 lines of code to execute.


----------



## Ryan360 (Jun 22, 2015)

MEBCWD said:


> When I first started using the curve fit tool I was surprised at how much time I did save cutting some of my files. I just offset vectors and never looked at them. One day I was editing a file and went to node edit some vectors and discovered I had a lot more nodes than I thought there would be.
> 
> As an example, using 2 lines 24" long and one has 2 nodes, a start point and an end point and the other line has 480 nodes equally spaced at 0.05" apart, the tollpath feed rate is set at 100 IPM.
> 
> ...



So i was messing around with the software (cut2d) and what your saying defiantly makes sense. When running about 70ipm i could clearly see that the quick "jitters" was from a node. So im guessing you can't get away from that unless you have 100% acceleration? Or would having better stepper motor drives/interface help with that?
thanks!


----------



## MEBCWD (Jan 14, 2012)

Don't forget about your post processor as 4D pointed out it will have an out come on the way it writes your gcode. It can use different values to produce the gcode file depending on how tight the tolerances need to be for a give toolpath. With a zero value it writers the gcode so the toolpath will have to run from node to node with no deviation. When given a value for the tolerance the post processor will try to adjust the code for the best cutting solution holding to the tolerance given so the cut won't be from node to node but will be as close as possible within the tolerance given. You will still have the start and stop to load the next line but the number of lines of code will be reduced so the code will run faster. 

If you examine most standard post processors for cutting 2d toolpaths and post processors for 3d toolpaths you will see that the 2d post processors usually hold a closer tolerance than a 3d toolpath. With all the moves that a 3d carving makes a close tolerance would build a much longer gcode file. By using wider tolerances for the 3d file the gcode will be written to smooth out movements the machine needs to make to cut a good representation of the item but limit the time needed.

If the curve is optimized for the least number of nodes and the post processor is given a value for a tolerance to hold you will get the best of both worlds, because the gcode will be adjusted for the best cut. The same can be said for a 3d model, if it is smoothed (or optimized) before running your toolpath and you use the proper post processor it will give you the best carving versus time gcode file.


----------



## Ryan360 (Jun 22, 2015)

MEBCWD said:


> Don't forget about your post processor as 4D pointed out it will have an out come on the way it writes your gcode. It can use different values to produce the gcode file depending on how tight the tolerances need to be for a give toolpath. With a zero value it writers the gcode so the toolpath will have to run from node to node with no deviation. When given a value for the tolerance the post processor will try to adjust the code for the best cutting solution holding to the tolerance given so the cut won't be from node to node but will be as close as possible within the tolerance given. You will still have the start and stop to load the next line but the number of lines of code will be reduced so the code will run faster.
> 
> If you examine most standard post processors for cutting 2d toolpaths and post processors for 3d toolpaths you will see that the 2d post processors usually hold a closer tolerance than a 3d toolpath. With all the moves that a 3d carving makes a close tolerance would build a much longer gcode file. By using wider tolerances for the 3d file the gcode will be written to smooth out movements the machine needs to make to cut a good representation of the item but limit the time needed.
> 
> If the curve is optimized for the least number of nodes and the post processor is given a value for a tolerance to hold you will get the best of both worlds, because the gcode will be adjusted for the best cut. The same can be said for a 3d model, if it is smoothed (or optimized) before running your toolpath and you use the proper post processor it will give you the best carving versus time gcode file.


Ok, i will have to look into the post processors, i know cut2d gives a bunch of them, i just usually go with something like ARC mach3 Inch.....i just use that one because im using mach3, and working in standard units. But maybe the "ARC" stands for something im not familiar with.
thanks for your help so far!


----------



## MEBCWD (Jan 14, 2012)

Ryan360 said:


> Ok, i will have to look into the post processors, i know cut2d gives a bunch of them, i just usually go with something like ARC mach3 Inch.....i just use that one because im using mach3, and working in standard units. But maybe the "ARC" stands for something im not familiar with.
> thanks for your help so far!


You will want to use the post processors that were written for your machine control software (ARC mach3 Inch) but you can edit these post processors to change the tolerance values if you chose to have a closer or looser tolerance. If parts you cut are not fitting together well and the CNC is producing a smooth cut then you might need to change the tolerance values.

I think the important thing to consider is optimizing the vectors so you have the fewest number of nodes for the post processor to deal with when generating the gcode file.


----------



## subtleaccents (Nov 5, 2011)

I didn't see where you posted the material you were cutting, the thickness of the material, the spindle speed and feed rate.
When I first got my machine the power supply that controls the spindle speed was incorrectly programmed at the machine manufacturer and the spindle speed was much lower that what the program was set for. This caused a bad vibration when I was cutting the 1/2" thick Corian, or any other material I tried to cut.


----------

