Machsupport Forum
Mach Discussion => Mach4 General Discussion => Topic started by: dq828 on September 23, 2017, 07:34:32 AM
-
Ivé had this issue both times I have cut something when the original Fusion Sketch was drawn with Spline Lines. The issue being, the Feedrate changes a lot during the cut. When the cutter is cutting the peaks of the knobs in the attached image it runs at the correct feedrate, when the cutter gets half way into the valleys, the feedrate slows to about 1/5 of the set feedrate and jerks forward until it is half way out of the valley and then it speeds up again, repeating this over and over as it goes around. Very annoying
Does anyone know what might cause this erratic behaviour, if anything I thought it might slow down on the tighter peaks?
At this stage I dont know much about code and rely on Fusion Cam to do it for me. I have just had a look at the code and there are sections throughout that look odd to me, see below, maybe you can tell me whats going on.
-
There are no splines in G- code so all moves get converted to arcs and short lines. So if you have exact stop programmed the machine will start and stop for every line segment making for rough motion.
-
dq838,
You must use CV to reduce machine shake.
Selecting the correct CV will produce outcomes very close to your profile.
If your machining at between 400mm to 1000mm per min, set all the CV 180 angles from 0 to 100.
Regards,
Mauri.
-
Thanks for the reply's.
I set CV and the CV angles a while back (from your advice) to overcome the Wonky Cutting issue, so I dont think it could be causeing this issue.
-
dq828,
Yes, you are correct you have CV running, I did not fully read all your notes until now.
The slow down is the angles and the CV in action.
As you do not show us the exact full F speed I cannot confirm weather the CV is set correctly.
Please advise the F speed and the CV setting, the cutter type and size and the material type being machined.
With this info, I may be able to provide a more optimal set of settings to perform your job.
Using Exact Stop will do the task correctly however will take longer.
Jerkiness is also caused by going too fast and your machine is not built to handle these speeds and directional movements.
Regards,
Mauri.
-
The Feerate is 1000,
The cutter is a 1/4' 2 flute carbide wood bit.
I am cutting plywood and only about 1/4"deep each pass
The CV angles are all set to 100
The bit I dont understand is the code that cuts the tops of the peaks, which has much tighter curves looks like this;
G1 X70.556 Y156.473
G2 X70.605 Y156.572 I2.863 J-1.372
G1 X70.944 Y157.221
G2 X70.979 Y157.286 I2.814 J-1.471
G1 X71.349 Y157.955
G2 X71.369 Y157.99 I2.779 J-1.536
G1 X71.76 Y158.678
When this type of code runs it all works fine and runs smoothly
And the code that cuts the shallower valleys looks like this, and it's where the jerkyness is, and the Spline line is all one continuos line;
X71.764 Y158.684
X72.566 Y160.086
X72.943 Y160.769
X73.298 Y161.445
X73.623 Y162.108
X73.919 Y162.772
X74.042 Y163.073
X74.16 Y163.385
Is there anyway to enter the CV angles in bulk, rather than one at a time!
-
dq828,
It looks like you are using a Router Table and probably have single one direction rails.
If you had rails also in the other direction it would stop any kicking "jerkiness".
So on some angles it probably depends on the direction of movement more X then Y making it Jerk more on the X axis than the Y axis.
You can slow down the F speed to compensate or reduce the CV settings.
Or if you can affix a Roller under the Router Table to stop the X axis kicking that would eliminate your problem.
Two was of setting CV on all axis.
If you do not change the Mach 4 Settings you could make a set of machine.ini with different CV settings.
You can manually edit the machine.ini in notepad make a Set 100 then save it as machine100.ini.
Then make a CV 75 and CV 50 and save it as machine75.ini and machine50.ini etc.
When you want to use a specific one your copy one into another directory and rename it to machine.ini and put it back inti Mach4 directory replacing the existing one (make sure you copy it back and rename it back to machine*********.ini.
When you make the changes in notepad do a search for say = 75 if only the CV angles are 75 and you want 50 then do a replace all.
Hope this helps.
Regards,
Mauri.
The other method is if you know Lua you could code it up on a Mach4 Screen to do it on the fly automatically.
Regards,
Mauri.
-
Your two code examples, the first the Cam program was able to generate lines and arcs so the motion is smooth. Then the spline curves could not be done using arcs so it made lots of tiny lines to approximate the curve and that motion is jerky as a result.
-
Yes, but it's all one Spline line, not an arc and then a Spline, as you say the CAM just couldn't do it all as arcs, I'm sure there is some geometric reason for this but it is beyond my knowledge.
I did manage to speed it up by increasing the CV angle speeds and making the Smoothness setting in Fusion coarser.
I thought I'd out smart the program but using the Spline on the peaks and then an actual arc in the valley's but of course Fusion then refused to generate a toolpath !!!
All good fun and learnings
Thanks for the help
-
One last question, I'm assuming that with the CV angles, 1 degree is basically the tightest angle, and 179 degrees is the shallowest angle, is this right.
I would have thought the best thing to do with the angle speeds is have the slowest speed required to cut the tighest angle, and then gradually increase the speeds as the angles get shallower.
I am amazed that one cannot copy and past into the CV Wizard table.
-
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.
-
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.
-
Thanks for the input, I get the theory even though I dont understand the Maths, it'll be trial and error for me.
-
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.
-
Chaoticone,
Yes that would be of interest to many of us.
Regards,
Mauri.
-
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.
-
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
-
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?
-
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
-
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.
-
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.
Don't hold your breath then. Without some putting in their time (I guarantee you setting up an inch profile for a machine is way faster than writing this wizard) to do some real world test and give results in inch I highly doubt I will spend any more of my time adding metric.
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?
Absolutely not. Setting the max speed any angle will go at to hold a tolerance has nothing at all to do with the feed rate you program. If your programed feed rate is lower than it can take the angle at....... it simply doesn't slow down because it doesn't have too to hold the tolerance. The speed capable does not in any way speed the feed rate up over the programmed feed rate. It will simply lower the speed in angles it needs too, it will never speed it up over programmed feed rate.
The angle is measured from current trajectory to next trajectory. Simply the difference of what it is doing now to what it will do next.
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 Configuration Menu. So the way I see it is selecting Constant Velocity in the Configuration menu actually does nothing unless you change the settings in the Wizard, is that right?
Not exactly but enabling CV in general config. does not populate the CV_Feed rate table in any way, therefore you are not taking advantage of that added feature until you populate the table.
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
You can populate the table any way you want, what ever works for you. That is kind of the way the last version works. I can't imagine a scenario that this version is not far superior though. This version is much smarter.
-
Chaoticone,
Thanks for your reply.
Are the CV values generated by your program changed to Integers?
If we convert the Imperial version to Metric do we need to change them to Integers or leave them in decimal form?
Is this curve generated by your CV program a form of a Polynomial?
Regards,
Mauri.
-
No problem
No, no conversion to integers. They begin as integers and end as integers. I suspect if I wanted to add resolution they could very well end as floating point but i don't see the need for that. Never heard of anyone programming a feedrate as a floating point but that doesn't mean it would necessarily be illegal to do so but it might be. I haven't ever given it enough though to know for sure one way or the other TBH.
I think I would convert to integers just to play it safe.
Well, I use polynomials to get there. But I also use tables and conditionals but most of it is polynomials I guess.
-
I too work in mm, so have been reading this post with interest and have had a look at the document that Mauri uploaded.
I haven'd installed the wizard onto my machine yet, but have a question about the output into the table. For instance take the following output generated in inches.
Angle_100=6.000000
Angle_101=6.000000
Angle_102=6.000000
Angle_103=5.000000
Angle_104=5.000000
Angle_105=5.000000
Would I input values into my table as such for metric?
Angle_100=152.4
Angle_101=152.4
Angle_102=152.4
Angle_103=127
Angle_104=127
Angle_105=127
-
Allen,
Yes all you have to do is multiple the CV Imperial values by 25.4.
Then Copy them into the machine.ini.
To make it easier for you to do this:
Copy Angle_0=x.****************** to Angle_179=x.****************** into Excel.
Then use Replace to change Angle_???= to blank you will have to do this 3 times Angle_?= then Angle_?? and Angle_???=
Then multiple all 180 value by 25.4.
On another column enter Angle_1 and then on the next 2 lines Angle_2 and Angle_3.
Then highlight the 3 and double click the dot on the bottom right hand corner of the highlight this will make a column from 0 to 179.
Next on another column make a column of =
Finally copy the column of you metric values to the right of the = column.
Then copy all the 3 columns and replace the one in machine.ini be selecting Paste Special Text .
Then fire up Mach4, followed by exit.
Save this file line machine2A00254.ini meaning 2 axis .00254mm error or any equivalent tolerance conversion for .1 to .0001 to metric.
By doing this the tabs will disappear in the machine.ini copy that you made and all the Angles, =, numbers will come together.
You can make multiple sets with other combinations of Axis and Tolerance.
So every time you want another type click open in notepad and save it as machine.ini.
Hope this helps to make it easier.
Regards,
Mauri.
-
Allen,
I forgot to mention make the numbers column in excel numbers with 0 decimal that way they will roundup to the nearest Integer value.
Regards,
Mauri.
-
Guys, I hope to have a version that will work in machine setup units (inch or metric) later tonight or tomorrow.
I hope this wizard will eliminate the need for multiple setups. If job tolerance changes or job type that changes axis involved, just run the wizard.
-
Excellent thanks
-
Here you go...... this update populates the CV_Feedrate table in inch or mm and the tolerance you enter is inch or mm........ all dependent on machine setup units.
Let me know how it goes.
-
Chaoticone,
That is much easier, thanks.
It seems to follow the profiles very well on small .01mm cut profiles, tested many different types in simulation.
I will run some controller tests soon and compare process times on some profiles your system vs our all angles the same version.
Regards,
Mauri.
-
Good deal. thanks!
-
Hopefully this will be the last update.......... no functional difference. I just added the blend radius for each angle to the ini and the CV_Feedrate table so 2 files here.
-
Thats excellent thank you, I've learned and gained a lot from this thread.
Last weekend I was trying to cut some timber clamp knobs and the cutting was very slow and jerky, I have just run a test with the knowledge and Wizards I have got from this thread and it runs as smooth as silk.
Once again thankyou.
-
Chaoticone,
I did a lot of testing last night and this morning on lettering 2mm upper and lower case engraving a standards on brass engravings.
2 Axis selected using CV program vs all angles the same.
The Doc attachment below contains all my findings.
The first main issue that I have found is that the Mach4 program has a flaw in the CV area, in that when you go from G1 to G0 it goes off line.
If you make all the code G1, then it does not, but the time increases significantly.
The second issue on lettering is that no matter the tolerance setting on your CV program on curves it does not follow the line.
Two items affect this:
1) CV being to high on some Angles
2) The change from higher CV to lower CV.
I have provided all combinations in my DOC file with screen capture examples.
On 3D engravings and continuous line engraving it has less of an issue and the CV program works well.
Regards,
Mauri.
-
Thats excellent thank you, I've learned and gained a lot from this thread.
Last weekend I was trying to cut some timber clamp knobs and the cutting was very slow and jerky, I have just run a test with the knowledge and Wizards I have got from this thread and it runs as smooth as silk.
Once again thankyou.
Good deal!
-
The first main issue that I have found is that the Mach4 program has a flaw in the CV area, in that when you go from G1 to G0 it goes off line.
This is no surprise. There is no CV in Rapids (G0). Rapids are well rapid, no throttling back. Get there as fast as your motor tuning will allow.
If you make all the code G1, then it does not, but the time increases significantly.
I would imagine it does. This would be equal to starting a round track race and telling car number G0 he just has to get to the other side and can drive through the infield (shortest path) while telling car G1 he has to stay on the track.
The second issue on lettering is that no matter the tolerance setting on your CV program on curves it does not follow the line.
I fully expect that. The question is, does it stay within the tolerance you entered? If so, that's the best that can be done with CV. If you have to stay exactly on path then CV is not an option. That is what exact stop is for.
-
Chaoticone,
Thanks for the reply.
I decided to make one more test.
Instead of calculating an optimized G-Code on all the lines at once, I decided to do each line separately in Rhino/madCAM and optimize each line separately, but output it as one G-Code.
I tested one with CV .001mm Tolerance and the other all Angles at 100 keeping the G1 and G0 as is.
This method no longer has the off line movements on going from G1 to G0, but does takes a bit more time, however a lot less than all G1.
So for lettering this is the way to go.
The result in the DOC.
Regards,
Mauri.
-
CV in CNC applications is an interesting subject and there are many out there that have been studying this issue for some time.
Here are some more mathematical ways of making a angle to a tolerance at maximum speed.
Regards,
Mauri.
-
Had a look at those papers but it makes my head hurt.
-
Hi,
yeah, but hurt in a good way LOL. That last paper that uses a cascade of FIR filters looks like 'just the dogs dangly bits'
Overlapping two motions with a constrained error term...just brill...there are some very sick little puppies out there!
Craig
-
I'm pretty new to Mach4 so forgive me if this is obvious to everyone but me. I don't want to break anything on my setup so I'm perhaps being overly cautious.
Right now I just have CV turned on in the main Mach4 config. Not in the CV Wizard. Am I correct in assuming that this will provide a generic CV profile that Mach will use?
When I install the 2 files that Chaoticone provided into the Mach4 Wizards folder and run it like any other wizard it will populate the Wizard CV table with more optimised settings based on what I input, and if I check "Use CV" here then it will use these figures? If I uncheck the box then it goes back to the generic CV from the main Config?
Is it advised to copy my profile and work with the copy when I'm doing something like this?
-
Right now I just have CV turned on in the main Mach4 config. Not in the CV Wizard. Am I correct in assuming that this will provide a generic CV profile that Mach will use?
Not really, the only thing that setting does in general config is set the default mode to CV or exact stop. When you fire up Mach or click the reset button it sets things to a default state. In regards to this, it activates default modal codes (G64 or G61).
When I install the 2 files that Chaoticone provided into the Mach4 Wizards folder and run it like any other wizard it will populate the Wizard CV table with more optimised settings based on what I input, and if I check "Use CV" here then it will use these figures? If I uncheck the box then it goes back to the generic CV from the main Config?
Not necessarily. To use the values generated by the wizard the api call mc.mcMotionSetCVAngleEnable has to be called. When you go through the mcCvTuningWizard this call is executed to enable it. In the CV_Feedrate wizard (table) you can enable or disable it by toggling the button up top. I can't think of a reason anyone would want to turn it off (because exact stop mode ignores it all together anyway) but good there is a call to control it through script if you had a need to.
-
Is any of this information written in a Manual somewhere, seems like very important info to me?
-
Hi dq282,
regrettably manuals always seem to be some years behind the forefront of Mach4. This does cause lots of consternation but that's the way it is
and unless Artsoft start charging us bigtime its not going to change dramatically for a good while yet.
On the other hand your original post and all the replies, ancillary questions and comments are all available for anyone to follow. The forum IS
the manual.
Craig