It is currently Mon Jun 18, 2018 3:20 pm

 

Help with possible settings mach3 and sheetcam. Pause at change of feed rate

Mach 3 CNC from Artsoft questions or tips can be posted to this forum.
User avatar
AdrianH
Elite Contributing Member
Elite Contributing Member
Posts: 75
Joined: Tue Dec 27, 2016 1:08 pm
Location: Blackburn England
Contact:

Help with possible settings mach3 and sheetcam. Pause at change of feed rate

Postby AdrianH » Sat Jul 08, 2017 9:57 am

As I am not sure where this should go for the time being I will leave in the general section and a mod could move it to the correct section if it goes one way or the other.

I have a complete home made system, done very cost effective, but is a small machine. I am learning as I go trying to pick up things the best I can.

I have put a few cutting rules in Sheetcam just to see the effects it has when cutting. Now I am only cutting thin metal 1.5 mm so probably need very little, but some the cutting rule will slow down the feed rate to 80% going into a sharp corner and speed up going out etc, but what I am seeing when cutting is what looks like a pause as mach3 changes feed-rates during the cut, almost like it decelerates and then speeds up again when changing feed-rate.

Now I know the computer is not the fastest but it does seem to deal OK, I have CV switched and on looking ahead 50 lines, I have also tried with Plasma Mode on and off, I have made sure that within Mach3 general config the setting for 'stop CV for angles > is switched off, as the idea I would assume is to use the rules instead.

So have I missed something that is causing these apparent pauses?

Is it the normal thing for it to do this?

Lastly at what metal thickness’s would you start to use these type of rules, thin metal or thick metal and what settings.
I would really appreciate your knowledge.

Thanks
Adrian

tcaudle
Posts: 972
Joined: Tue Feb 28, 2012 6:47 pm

Re: Help with possible settings mach3 and sheetcam. Pause at change of feed rate

Postby tcaudle » Sat Jul 08, 2017 2:48 pm

No machine can instantly switch speeds. Its up to the acceleration curve of your setup. It DOES have to decelerate and accelerate when switching speeds. You may find that if you want to use rules you need to retune the motors to more gently make the transition. Of course that makes it so you HAVE to use rules on corners and sharp turns because MACH's trajectory planner favors speed over tracking (toolpath) . CV tries to hold as close to the commanded speed as it can and it will "fudge" turns and either round them off or cut across at an angle. The longer the acceleration curve the more it deviates. If you use the CV settings to have to switch

from CV to exact stop ti will then adhere to the toolpath but does not do lines with multiple nodes well. The speeds of the computer is not a factor in this. If its a parallel port system, all it has to do is be able to generate the pulses fast enough to go the speeds (max velocity). Its true that the parallel port has "jitter" and its worse at lower kernel speeds. Jitter is what tends to cause motor stalls in steppers at a lower RPM than a smooth waveform.

User avatar
AdrianH
Elite Contributing Member
Elite Contributing Member
Posts: 75
Joined: Tue Dec 27, 2016 1:08 pm
Location: Blackburn England
Contact:

Re: Help with possible settings mach3 and sheetcam. Pause at change of feed rate

Postby AdrianH » Sat Jul 08, 2017 3:08 pm

Sorry, perhaps my description of what I saw and thought is a problem was poor. I will try to explain a bit better, and I will put it in inches rather than metric.
my cutting rule is something basic such as this
When cutting in a straight line the feedrate is 90 IPM (100%), when it is within 1/4 inch of a sharp bend it should reduce to 80% so 72 IPM. 1/4 inch after the bend back to 100% so 90 IPM.

Now I guess what I was expecting to see was at 1/4 inch before it decelerates down to 72 IPM perhaps taking an 1/8 inch, go around the corner at 72 and at 1/4 after accelerate back up to 90 again taking about1/8 inch.
But
What I appear to be seeing is a dead stop, in that before the 1/4 point it decelerates from 90 to 0 and then at the 1/4 mark accelerates up from 0 to 72.
Same coming out of the corner
So at the 1/4 before and 1/4 after I am now getting divots as the arc stops. I will go and get the cut metal out of the scrap bin and take a picture with the rules and without.

What happened to the motoguy post?

Adrian

User avatar
AdrianH
Elite Contributing Member
Elite Contributing Member
Posts: 75
Joined: Tue Dec 27, 2016 1:08 pm
Location: Blackburn England
Contact:

Re: Help with possible settings mach3 and sheetcam. Pause at change of feed rate

Postby AdrianH » Sat Jul 08, 2017 3:36 pm

withrule.jpg


With rule


withoutrule.jpg


Without rule.

I did not clean up the first cut pieces just throu them in the bin so the second one has a bit of time in the vibratory tub before that decided to trip the mains :(

The actual rules on these come in at something like 3mm before and after so around 1/8 inch.

Adrian

You do not have access to download this dxf file.
Become a Contributing Member to gain access to the thousands of files shared by our members. Click Here


motoguy
Posts: 1054
Joined: Tue Aug 25, 2015 12:05 pm
Location: Central MO, USA

Re: Help with possible settings mach3 and sheetcam. Pause at change of feed rate

Postby motoguy » Sat Jul 08, 2017 3:43 pm

I used to have this issue as well, with my Mach/Windows controller. I was running something like 40-45ips^2 accel rates on my Bulltear/Starlab table.

Same thing as you, at the "transition point" my torch would have a little "hiccup", resulting in a small divot entering and exiting the corners. The only way I could make it go away was to run with CV shut off, and no rules. However, then I started rounding all my sharp corners, and my shapes went to hell. I could leave CV off, and use cut rules to slow down at corners, but I'd have to slow down well before the corners, and even then the CV rules would sometimes blow the shape (at 225ipm on 14ga, even 50% reduction is still 112 ipm, which would lose some sharp corners).

I ended up just leaving CV engaged, and dealing with the small notch/divot coming into/out of corners. This was one of my main complaints with the Mach/Windows setup, and one of the many reasons I wanted to go to the Linux/CommandCNC setup. Since going to Linux/CommandCNC, this issue has gone completely away. Along with needing to use a lot of cut rules, worrying about crashing all the time, etc.

If you can swing it, I suggest upgrading from Windows/Mach to Linux/CommandCNC. It really is much much better. Even dross seems reduced with Linux. I used to run a standard .1 overcut on 14ga, to have a clean exit. With Linux, I'm now down to running a .03 overcut (1/2 kerf with), and the lead in/lead out point is much cleaner.
Bulltear 6x12 w/ Proton Z axis & watertable
CommandCNC/Linux w/ Ohmic & HyT options
Hypertherm Powermax 85 w/ machine torch
Solidworks, Coreldraw X7, Inkscape, Sheetcam

motoguy
Posts: 1054
Joined: Tue Aug 25, 2015 12:05 pm
Location: Central MO, USA

Re: Help with possible settings mach3 and sheetcam. Pause at change of feed rate

Postby motoguy » Sat Jul 08, 2017 3:46 pm

AdrianH wrote:Without rule.

I did not clean up the first cut pieces just throu them in the bin so the second one has a bit of time in the vibratory tub before that decided to trip the mains :(

The actual rules on these come in at something like 3mm before and after so around 1/8 inch.

Adrian


My Mach controls always had a small pause in motion when rules activated/deactivated. Usually this was a slowdown and deactivation of THC for corners, circles, or some other shape. Sometimes it was just deactivation of THC. HOWEVER, in order to SEE where the THC deactivated in Sheetcam, I would often change the feedrate to 99% (feedrate changes show up in sheetcam as different colored lines, making it easy to see where the rule would be on/off.) So, I'm not sure if ANY rule creates a hiccup (something like disabling THC only), or if it's rules that change feedrates (slowdown for corners, arcs, shapes, etc).

The thicker the material got, the less noticeable it was. Probably the combination of more metal to need to melt, as well as slower transition rates due to slower feedrates for thick material. The "dings" could get pretty noticeable on 14, 16, 18ga though.
Bulltear 6x12 w/ Proton Z axis & watertable
CommandCNC/Linux w/ Ohmic & HyT options
Hypertherm Powermax 85 w/ machine torch
Solidworks, Coreldraw X7, Inkscape, Sheetcam

User avatar
AdrianH
Elite Contributing Member
Elite Contributing Member
Posts: 75
Joined: Tue Dec 27, 2016 1:08 pm
Location: Blackburn England
Contact:

Re: Help with possible settings mach3 and sheetcam. Pause at change of feed rate

Postby AdrianH » Sat Jul 08, 2017 5:05 pm

Thanks for the responses, perhaps it is Mach doing a few things, I also turn off THC in corners or arcs etc, in the pics below this is not a corner really because I tend to round the corners a 1/16" or so to stop a divot point in the absolute corner. So the below is on detection of an arc, but the same rules as corner.

What I wanted to figure was if I had something else wrong in the config. When would you consider needing cut rules with at what thickness of sut would you consider it, I was just going to start thin and slowly over time work thicker, but if the issue I have is not a wrong config, then I may well skip the idea.

I have thought many times about LinuxCNC as I run a few PC's on Suse Linux, the one I am typing on now is one in fact. Are you running the real time kernel?

Cheers
Adrian

Forgot to say, my baby plasma table on 1.5mm was cutting at 27 Amps at 86 inch per min accel is only 18 inch per sec sec. So possibly a reason why I am seeing it more noticeably.

tcaudle
Posts: 972
Joined: Tue Feb 28, 2012 6:47 pm

Re: Help with possible settings mach3 and sheetcam. Pause at change of feed rate

Postby tcaudle » Sat Jul 08, 2017 8:34 pm

It depends on HOW you are turning off the THC. Doing it with a macro (custom Mcode) will cause motion to stop until the macro executes. If its in the Gcode as an M code it executes code one line at time and does not swtich to the next line until the engine senses the line has completely executed.

The only way to do it is to have a THC that you can turn on and off with some form of G-code that does not have to finish executing to keep running motion.

Linuxcnc has two forms of commands . One is a statc command and the other is a dynamic command that executes in during the next motion move so it never stops

Rodw
Posts: 122
Joined: Sun Aug 21, 2016 1:49 am

Re: Help with possible settings mach3 and sheetcam. Pause at change of feed rate

Postby Rodw » Sun Jul 09, 2017 4:12 am

I think plasma is a bit like driving a car. You can't go into a 90 degree corner without slowing down and even then you can't follow the line you wanted exactly. But if you have an old crash gear box in your car, you can't change gears without stopping.

Really you are coming up against limitations of the Windows OS as it is not real time. That is the reason why Tom and a number of other commercial companies have moved from Mach to LinuxCNC which is a real time system that guarantees that things happen 1000 times a second every millisecond on time every time (on a properly configured system).

Linuxcnc will give you an upgrade to a synchromesh gearbox so you don't have to stop to change gears but there isn't a plug and play system for plasma yet. (although you can import your Mach 3 config in a few minutes).

If you just want to get cutting, one of Tom's packaged systems is the way to go. If you want to stay a DIY kind of guy, you can get LinuxCNC to do plasma. Its taken me 12 months and I'm nearly ready to cut something. i've shared a lot of my journey here http://plasmaspider.com/viewtopic.php?f=103&t=22826 and on the LinuxCNC forum (where I delve a lot deeper into putting the pieces together). Hopefully the next guy will have an easier journey.

User avatar
AdrianH
Elite Contributing Member
Elite Contributing Member
Posts: 75
Joined: Tue Dec 27, 2016 1:08 pm
Location: Blackburn England
Contact:

Re: Help with possible settings mach3 and sheetcam. Pause at change of feed rate

Postby AdrianH » Sun Jul 09, 2017 6:04 am

Thanks again for your answers and I believe it tcaudle probably got it because the THC off in my little system is a macro.

And here are the lines of code that sheetcam generated around one of the pauses in cutting

N6060 M102 (On arcs)
N6070 G01 X314.1213 Y180.5000 F2200.0
N6080 M101 (On arcs)
N6090 G01 X311.1213 Y180.5000 F1760.0
N6100 G02 X308.6213 Y183.0000 I0.0000 J2.5000
N6110 G01 X308.6213 Y187.0000
N6120 G02 X311.1213 Y189.5000 I2.5000 J-0.0000
N6130 G01 X314.1213 Y189.5000
N6140 M102 (On arcs)
N6150 G01 X344.6213 Y189.5000 F2200.0
N6160 M101 (On arcs)
N6170 G01 X347.6213 Y189.5000 F1760.0
N6180 G03 X348.6213 Y190.5000 I0.0000 J1.0000
N6190 G02 X350.6213 Y192.5000 I2.0000 J-0.0000
N6200 G01 X353.6213 Y192.5000
N6210 M102 (On arcs)
N6220 G01 X423.1213 Y192.5000 F2200.0
N6230 M101 (On arcs)
N6240 G01 X426.1213 Y192.5000 F1760.0
N6250 G02 X429.6213 Y189.0000 I0.0000 J-3.5000
N6260 G01 X429.6213 Y186.0000
N6270 M102 (On arcs)

M102 is turning the THC on and M101 turning it off as it slows down, so if these are briefly pausing things then there is my issue.

I will experiment to prove it by basically not turning the THC off on arcs. it is good to figure reasons why it does not perform as expected.

I do appreciate I could buy a ready made system and have all the problems sorted for me, but I like to learn, figure out and also post my journey for others. the idea is they don't go through the failures.

But in my little work area here in the UK I have a bench top, so built a bench top system, it cost me in parts probably less than $1,000 total, the hours are probably in the hundreds if not thousands by now, but it keeps my brain working and as I am not doing any commercial work for others has to do as it does not provide any return.

Cheers

Adrian

tcaudle
Posts: 972
Joined: Tue Feb 28, 2012 6:47 pm

Re: Help with possible settings mach3 and sheetcam. Pause at change of feed rate

Postby tcaudle » Sun Jul 09, 2017 2:07 pm

No need to experiment. the parsing engine in MACH will stop and execute the command and wait until its finished.
The only M commands in MACH that do not cause a motion pause are M10 and M11. They are designed for laser control and will only control an Output. You can write a macro that is tied to an OEM output and directly turn the THC logic in MACH on and off. If you try to use an external real output you have to have a THC that can be enabled/disabled via an external signal. Those MACROS were written to use before or after a cut , not with cut rules.


Return to “Mach3 CNC”

Who is online

Users browsing this forum: No registered users and 1 guest

Easyscriber engrave attachment for Hypertherm torch's