It is currently Thu Dec 14, 2017 9:55 am

 

Anyone running UCCNC?

General software related questions should be posted here.
RAD
Posts: 73
Joined: Fri Aug 28, 2015 3:17 pm

Anyone running UCCNC?

Postby RAD » Sat Aug 19, 2017 5:52 pm

just curious if anyone is using ucCNC and what constant velocity settings you have set. I have switched from mach3 to unCNC, i am liking it so far but can't seem to get a consistent motion on corners the machine decel and accelerates on line segments of corners this affects cut quality a bit. I have cut the same part in mach3 an the cut quality is slightly better however i was surprised to see it had significantly more dross than when cut with ucCNC.
D.I.Y 4x4 CNC Plasma Table with water tray
60 Gal. A/C + D.I.Y Aftercooler + Water/Oil seperator + Desicant air dryer
45XP (CPC with hand torch)
MiniTHC
UCCNC + Sheetcam + Inkscape / AutoCAD

beefy
Posts: 1239
Joined: Fri Jan 18, 2013 3:19 am
Location: Melbourne, Australia

Re: Anyone running UCCNC?

Postby beefy » Sat Aug 19, 2017 9:53 pm

I'm noticing that on the PC screen in demo mode (no board connected, just doing test stuff). I can visibly see the toolpoint slow down before corners and speed up after them. However, this is just a fresh demo install without touching any settings. The accel/decel default settings may be down really low.

Have you tried upping your acceleration/deceleration levels much higher to see if it makes a difference.

I'd go to the Cncdrive forum for support: forum.cncdrive.com

I don't think many users here even know about UCcnc. What I can say is that I've heard a few users say its trajectory planner is far superior to Mach3.

If the dross is everywhere then that is not a Mach3/UCcnc issue. Just adjust the feedrate to get a relatively dross free cut. Have you definitely got your "steps/per" set up correctly so the feedrate should be the same in both systems.
8 x 5 water table
Powermax 1250 with Duramax torch
Candcnc MP3000 / Mach3
Sheetcam
Geomagic Design 3D solid modelling
Coreldraw X5

RAD
Posts: 73
Joined: Fri Aug 28, 2015 3:17 pm

Re: Anyone running UCCNC?

Postby RAD » Sun Aug 20, 2017 9:27 am

Thanks i have set up all the settings in relation to c.v mode as best as I can get it but as you said the problem maybe due to poor acceleration of my motors, tried increasing accel but they are at there limit (i need bigger motors)

I have imported my mach3 xml. file into uccnc so all settings are identical to mach3 including steps per and motor tuning settings, all i had to set was a safe z height (there's were 25 by default all i needed was 1.5")

I am glad i converted to uccnc things are way more responsive with regards to timing
D.I.Y 4x4 CNC Plasma Table with water tray
60 Gal. A/C + D.I.Y Aftercooler + Water/Oil seperator + Desicant air dryer
45XP (CPC with hand torch)
MiniTHC
UCCNC + Sheetcam + Inkscape / AutoCAD

robertspark
Posts: 37
Joined: Mon Jun 12, 2017 6:43 pm

Re: Anyone running UCCNC?

Postby robertspark » Fri Oct 20, 2017 3:49 pm

Is this thread still a flyer or is it now dead?

I'm using it.

Slowing down in the corners is to do with your settings X & Y max accel, steps per unit (potentially) and also the corner error max.

Adjusting these will reduce the slowdowns in the corners.

I can go into detail but not if I'm chatting with myself.

beefy
Posts: 1239
Joined: Fri Jan 18, 2013 3:19 am
Location: Melbourne, Australia

Re: Anyone running UCCNC?

Postby beefy » Fri Oct 20, 2017 5:47 pm

RAD wrote:I have imported my mach3 xml. file into uccnc so all settings are identical to mach3 including steps per and motor tuning settings, all i had to set was a safe z height (there's were 25 by default all i needed was 1.5")

I am glad i converted to uccnc things are way more responsive with regards to timing


Same here.

Was happy to find a new Windows based solution where all the critical timing is done in the external motion controller. Many users report the motion planner is very smooth. Development is also ongoing.

It's relatively easy to program macros too and has a built in screen editor.
8 x 5 water table
Powermax 1250 with Duramax torch
Candcnc MP3000 / Mach3
Sheetcam
Geomagic Design 3D solid modelling
Coreldraw X5

RAD
Posts: 73
Joined: Fri Aug 28, 2015 3:17 pm

Re: Anyone running UCCNC?

Postby RAD » Tue Oct 24, 2017 12:01 pm

robertspark wrote:Is this thread still a flyer or is it now dead?

I'm using it.

Slowing down in the corners is to do with your settings X & Y max accel, steps per unit (potentially) and also the corner error max.

Adjusting these will reduce the slowdowns in the corners.

I can go into detail but not if I'm chatting with myself.


Thanks, I have managed to adjust the settings to the best that my motors can do, my motors are a bit undersized though.
I would appreciate if you can go into detail on the C.V settings, since I was adjusting mines by trial and error
D.I.Y 4x4 CNC Plasma Table with water tray
60 Gal. A/C + D.I.Y Aftercooler + Water/Oil seperator + Desicant air dryer
45XP (CPC with hand torch)
MiniTHC
UCCNC + Sheetcam + Inkscape / AutoCAD

robertspark
Posts: 37
Joined: Mon Jun 12, 2017 6:43 pm

Re: Anyone running UCCNC?

Postby robertspark » Tue Oct 24, 2017 4:31 pm

What are your motor settings (max velocity and acceleration)?

How did you trial and error set them?

I suggest performance testing them with a dial indicator.
Basically put a dial indicator on the bed, fix it in position (I use a magnetic clamp) with some additional Magswitch clamps added given the acceleration and jolt (jerk) is quite high and can get very pronounced long before the steppers stall the belts actually slip.

Then I jog the machine Left onto the dial indicator (which offsets for any backlash), zero the dial indicator + machine, and then command the machine to travel 100mm to the right "G0 X100", change the machine mode to relative distance mode "G91", and then I load an run a simple programme which will send the machine back and forth say 100 times, like this:

Code: Select all

G0 X100
G91
M98 P200 L100
G90
G0 X0
M30

O200
G0 X250
G0 X-250
M99


At the end of the programme I'll check my dial indicator, and hopefully its the same as when I started.

I'll change the "X" to "Y" and even "Z" (although reduce the travel distance from 250mm!!)

create 3 test *.tap files to automatically test the axis.


When you are testing and setting your axis, what you are looking for is not the highest velocity, but the highest acceleration setting, to do this you need to consider realistically what plasma cutter do you have, what does its book settings require feedrate wise, and what material + material thicknesses do you intend to cut (more so if you are operating a budget cnc system with undersized motors and drives etc).

Lets say, you have a hypertherm powermax 45 (non XP) like me, and you intend to cut 1/8" (3mm) and 1/4" (6mm) plate.
Your problem on feedrate is really the 1/8" plate (~3mm) and more so if you occasionally intend to cut 1.5 to 2mm plate (like I do).

From the book specs, feedrates for mild steel are as attached.
https://www.hypertherm.com/Download?fileId=HYP109170&zip=False
So for example 1.5mm requires 8890mm/min feedrate with 45A consumables with the machine set at 45A or if I set the machine at 30A, I can drop the feedrate to 5680mm/min.

{with 30A consumables + machine set to 30A (+thinner kerf advantage), the feedrate would be 4450mm/min}

The target acceleration is about 0.3G (~3000mm/s/s or ~116in/s/s) for plasma... note... "target", nice to have.

The reason for this high number is centripetal acceleration (speed of cornering).
because small scale plasma cnc requires constant feedrate (or as close as possible) because we cannot (for the most part) control the cutting current we need to compenstate by keeping the feedrate constant.

Hence lets say the thinnest you intend to cut is 1.5 mm plate , the maximum velocity your machine needs will be 8890 mm/min, you can now tune your machine using the above gcode to try to increase the acceleration to the point that the steppers stall and then back it off a bit, given your machine won't require more than this (I would work on a round number though like 9000mm/min)

Lets say you get 3000mm/s/s acceleration, what does this mean?
besides that you can get up to full feedrate (8890mm/min) in ~0.05 seconds, it means that the distance for the acceleration is ~3.66mm
It also means that when you cut internal corners they will be rounded by a radius of 7.32mm
Which if you think about it is fairly good, but we can make it better!

Now you also need to consider the step size of your machine, mine is quite course, 20 steps per mm, therefore 1 step per 0.05mm.
At first this may just look course, but how fine do you "really" need it for plasma cutting (my drives are set on 10uSteps, recommendation is to NOT use anything higher than this).

I am a practical person the average human hair is 0.001mm, If I can cut my plasma cut part out with a tolerance of 50 hairs (1 step) I'm over the moon! Considering all I'm going to do is paint and weld the parts anyway.

As I've been learning jolt / jerk needs to be considered, which is best considered with steppers as the time it takes between steps... so when the first step lands, how long before the second step lands.... distance = 0.05mm, acceleration = 3000mm/s/s,
time = square root ( distance x 2 / acceleration )
time = 0.005773 Seconds (or 5.7735mSec)
This then puts jolt / jerk at ~520m/s^3 [3000/5.7735, use mm with mSec or meters with Sec]

The higher the jerk / jot, the more stress you are putting your machine under and the less likley you will be to achieve 0.3G (I can achieve more!, way more!, to the point belts slip at just below 1G, but then the jolt / jerk would become ~3073m/s^3 (about 6x greater jolt effect).
The more steps per unit you have, the higher the jolt will become.


Back to UCCNC settings, the settings that are important are highlighted in the attached screenshot

Most important .... corner error max AND linear error max.

Linear error max, do not set this below your machines step resolution because you will never get benefit from this setting which can be considered as a tolerance setting, the default setting is 0.03, which means that the trajectory planner will keep the linear error below this number when moving from one position to another, if like in my case you are happy with 0.05mm step resolution, then set it to that number and it will work fine. you can of course set the number higher like say 0.1mm but this then gives your part a 1/2 step part accuracy tolerance.
The manual explains this one very well with a diagram.

Corner error max is basically the maximum allowable radius between two linear (or arc) moves and affects the centripetal acceleration setting (i.e. it will limit the cornering feedrate because the acceleration is fixed with a linear acceleration profile).

the default setting is 0.03mm, so with our example above, with 3000mm/s/s acceleration the maximum velocity that we can have at a 90 degree corner will be 9.5mm/sec in order that the machine keeps to the 0.03mm radius tolerance..... (which is below my minimum step resolution of 20steps per unit or 0.05mm per step). This means that the machine must spend longer in the corners than is nessesary which will have the tendancy to over-burn in the corners because the machine has to slow down too much. also this is now really constant velocity, because it's been over constrained by a very tight minimum radius requirement.

The accepted feedrate adjustment for cutting holes of less than ~25mm diameter is 60%, so looking at this another way, if we accept that in the corners we will slow the feedrate to 60% of the linear feedrate and then adjust the corner error max accordingly we will now have much more constant velocity and will have limited the amount of overburn in the corners. Back to our 1.5mm MS example, feedrate at 8890mm/min, 60% feedrate is 5334mm/min (88.9mm/sec), this allows us to correct the Corner Error Max to 2.63 ( Vel^2 / Acc = Radius )

hence we accept that with a 3G acceleration setting and a feedrate of 8890mm/min, that in the internal corners, they will be rounded by a radius of 2.63mm (negligible in my eyes) and we get no over-burn.

An interesting point now is say we put 30A consumables on the torch, because we are doing artwork and want a better finish, same 1.5mm MS plate, feedrate is now 4450mm/min (as stated above), hence 60% allowable feedrate reduction in the corners is 2670mm/min (44.5mm/sec), hence our Corner Error max now becomes 0.66mm! very crisp corners in my eyes and we still have no over-burn.

I created a macroloop code here to automatically adjust the corner error max according to the set linear feedrate. The catch is DONT use a code snippet to slow the feedrate before the internal corners and speed it up after the corners as you are now doing this automatically as part of the machines settings dynamically.
http://forum.cncdrive.com/viewtopic.php?f=16&t=810

The macroloop will not affect you cutting holes, given your feedrate will be lower and you normally won't cut 0.66 mm radius holes in 1.5mm mild steel.... and I think a 5.26OD mm hole will still be a challenge in 1.5mm plate.

The kernal frequency is also denoted as you don't want to set it higher than you really need to as it may lead to lost (missed) steps by your stepper drives, especially if they are cheap / low cost ones.

If you list / email me your profile, I'll have a look at it for you and provide comments.

Hopefully this waffle is of use to someone.

If you've not understood it or want me to elaborate on anything let me know.

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


RAD
Posts: 73
Joined: Fri Aug 28, 2015 3:17 pm

Re: Anyone running UCCNC?

Postby RAD » Tue Oct 24, 2017 8:11 pm

My system is setup in inches.

Best i can get out of my motors are:
Velocity: 180 in/min & accel: 16 in/s^2 these numbers seem poor but they work based on my low feedrate & low amperage, i get acceptable inside corners.

Steps size of my machine is 0.038" (with gear reduction and microstepping) again poor numbers compared to your 0.05mm! (3251 steps per inch, 10:1 gear reduction, 1600 microstepping) *edited: This might be wrong I think this should have been 1inch/3251 steps = 0.0003"

My linear error max. is set to 0.03 (just under my machine step size of 0.038") i guess i should set this to 0.04?

My corner error max is set to 0.03. My feedrate for 1.5mm MS is approx 105 IPM which would give a radius of 0.19" (according to your formula: vel per sec ^2/accel) not factoring the 60% corner slowdown. Should this be set to 0.19?

Very interested in your macroloop and i don't normally use cut rules for corner slowdown so this would be great. I will check out the link!

Will email my profile. I know however my limiting factor are my motors but if i can optimize them further based on your advice of my cv settings that would be great.

Much thanks for the info you provided, i am sure this will help others who are new to UCcnc
Last edited by RAD on Wed Oct 25, 2017 1:30 pm, edited 1 time in total.
D.I.Y 4x4 CNC Plasma Table with water tray
60 Gal. A/C + D.I.Y Aftercooler + Water/Oil seperator + Desicant air dryer
45XP (CPC with hand torch)
MiniTHC
UCCNC + Sheetcam + Inkscape / AutoCAD

robertspark
Posts: 37
Joined: Mon Jun 12, 2017 6:43 pm

Re: Anyone running UCCNC?

Postby robertspark » Wed Oct 25, 2017 7:57 am

Do you have the specifications on your motors?
Amperage:
Resistance:
Inductance:

What power supply voltage are you feeding your drives?

Why are you running a 10:1 gear reduction ratio (how heavy is your gantry?, do you need the increased torque?)

RAD
Posts: 73
Joined: Fri Aug 28, 2015 3:17 pm

Re: Anyone running UCCNC?

Postby RAD » Wed Oct 25, 2017 12:35 pm

Motor specs:
Amperage: 2.3
Resistance: 2.5
Induction: 5.3

24V to my drives

Got the 10:1 planetary gerboxes real cheap, and already had the above stepper motors so mated them together and voila! I'm on the lookout for 3:1 or 5:1 gearboxes if the price is right but so far this combination is working fairly well going in eight months of use
D.I.Y 4x4 CNC Plasma Table with water tray
60 Gal. A/C + D.I.Y Aftercooler + Water/Oil seperator + Desicant air dryer
45XP (CPC with hand torch)
MiniTHC
UCCNC + Sheetcam + Inkscape / AutoCAD

robertspark
Posts: 37
Joined: Mon Jun 12, 2017 6:43 pm

Re: Anyone running UCCNC?

Postby robertspark » Wed Oct 25, 2017 4:21 pm

24 volts is very low (but it does depend on the spec of your drives though [hence the rest of this may be over-ridden by your drives not being able to handle more than 24V)

I don't know how much you know about electronics, but inductive reactance (XL) is basically another form of resistance, and the faster the signal changes (steps) the higher the inductance becomes which resists current flow and then will rob your motors of torque.
XL = 2 x Pi x F x L

Circuit impedence (Z) = Resistance (R) + Indictive Reactance + Capacitive Reactance (Xc)
There is is chance where XL = XC, and this is at resonance .... given capacitance in stepper motors + drive circuits is quite low, its quite hard to establish electrical resonace.

Lets look at estimating what Z could be as a maximum
24 volts / 2.3 Amps = 10.435 ohms.
We know that R = 2.5 ohms, so the highest that XL could be is Z - R, which is 7.935 ohms.
Given XL = 2 x Pi X F x L, and we know everything but F (frequency) we can calculate the maximum attainable frequency (pulse rate) to the drives.
F = XL / (2 x Pi x L [in Henry, not mH]) which is 238Hz (238 pulses per second), above this pulse rate the current will drop off (it has to), the way to correct for this is power supply voltage

There is a "rule of thumb" (don't know how it was arrived at) which is documented here that recommends that:
http://www.geckodrive.com/support/step-motor-basics/power-supply-basics.html
To figure out what the maximum power supply voltage should be, use the following formula with the motor’s inductance in millihenries (mH) used for the L value.
32 * SQRT( L ) = VMAX
Hence your stepper motors could handle up to ~74 Volts

edit: it may have come from here (last line) http://www.piclist.com/techref/io/stepp ... ctance.htm

lets say your drives can handle 48Volts, reworking the above formula

48V/2.3A=20.870 ohms (Z)
XL = Z-R= 20.870-2.5 = 18.370 ohms
F = XL / (2 x Pi x L [in Henry, not mH]) = 551.4 ohms

551.4 hz / 238 hz, means that "theoretically" you can whatever the performance at 24V supply voltage, you can expect that to be 2.3 times higher at 48Volts..

my recommendation before changing stepper motors.... change the power supply if your drives can handle it (what drives have you got? manuf + model).

I may have kind of overcooked my setup a little... it is fed by 50V AC (~70v dc equivalent), and my motors are 4.2A with digital programmable (tunable) drives, hence expect that you could increase your performance to maybe 300 to 360ipm, with a similar increase in acceleration by changing your power supply (in my opinion).

One curious thing that I noticed tuning my drives, I actually reached a point with the acceleration that if I backed off on the maximum velocity the acceleration could be increased slightly (this happened about 0.6G from memory where the drives error'd out when the max velocity was set at 14,400mm/min (567ipm), but by reducing the max velocity setting to slightly below 10m/min (394ipm) I could up the acceleration to about 1G before belts slipped, but the jolt (or jerk) experienced by the table was too great (I even sat on it trying to provide some weight to the table mass and it still swayed).

Like driving a sports car, it doesn't help it by driving it like you stole it every time you get into it, hence you know whats under the bonnet for when you need it.

(Its why I'm beginning to understand jolt + jerk and adjust the steppers to what is needed acceleration wise relative to the feedrate and not running to tight corner error setting when its not needed all of the time)

RAD
Posts: 73
Joined: Fri Aug 28, 2015 3:17 pm

Re: Anyone running UCCNC?

Postby RAD » Wed Oct 25, 2017 8:55 pm

Very useful info ^

My drives are 2M542 rated for 24v - 50v
similar to this:
https://m.ebay.com/itm/2M542-CNC-Steppe ... 0408.m2460

My PSU (Phoenix Contact) is actually adjustable from 22.5v to 29.5v (i just checked) I believe i have it turned up to just below 29.5v

I'd be happy if i can get 2.3 times the performance from my steppers based on your calculation using a 48v psu.
It might even be cheaper than buying stepper motors.
Will try this first.

Much thanks!
D.I.Y 4x4 CNC Plasma Table with water tray
60 Gal. A/C + D.I.Y Aftercooler + Water/Oil seperator + Desicant air dryer
45XP (CPC with hand torch)
MiniTHC
UCCNC + Sheetcam + Inkscape / AutoCAD

beefy
Posts: 1239
Joined: Fri Jan 18, 2013 3:19 am
Location: Melbourne, Australia

Re: Anyone running UCCNC?

Postby beefy » Thu Oct 26, 2017 2:33 am

Go to the Geckodrive website and study up on their technical info. It gives you a good grounding in steppers and what voltage power supply you'll need to get max rpm from your stepper motors.

So that I could get max speed, I ended up with a power supply around 80 volts. However, your stepper drives must also be rated for the input supply voltage or they end up fried.

Think of the motors as acting like a generator but pushing back in the opposite direction to the supplied voltage. As the rpm gets higher, the motors push back with a higher voltage, thus as rpm increases you need a higher voltage to overcome this "reverse voltage" and to "push" the current through the stepper motor.

Steppers run at a constant current and the motor data sheet should say what this is. You should be able to set this current via your stepper drives. Increasing the current above this rated value doesn't give much more torque but the extra current will cause a lot more heating.

Keith
8 x 5 water table
Powermax 1250 with Duramax torch
Candcnc MP3000 / Mach3
Sheetcam
Geomagic Design 3D solid modelling
Coreldraw X5

robertspark
Posts: 37
Joined: Mon Jun 12, 2017 6:43 pm

Re: Anyone running UCCNC?

Postby robertspark » Thu Oct 26, 2017 3:09 am

I'd be a little bit careful with the power supply selection for the drives and don't run them too close to their rated voltage. When I first started out I killed a load of drives, but I started out with cheap drives on the strategy of buy cheap buy twice in the end....

If you are in the us, antek make good power supplies for cnc, the problem with stepper drives as beefy has stated is back emf, especially when stopping the drives fast and this is the spike that normally kills drives.

From my experience, some manufacturers like rating their products should we say optermisticaly ... Hence driving them to the limit of their voltage and or current rating leads to a short life.

The toroidal transformers tend to be best for.cnc
http://www.antekinc.com/power-supplies/
Switch mode power supplies are not recommended.

If you decide to change your drives, I recommend leadshine am882h drivevs (must have H on the end of the ref or they are std DC drives) as you can feed them AC as they have their own internal bridge rectifier and capacitors in them so all you do is get a toroidal transformer and connect it up to the drives. Unfortunately the am882h drives are no longer made but are sold cheap on eBay or aliexpress second hand from China or Taiwan as refurbished, I've bought quite a few and not had a bad one yet (touch wood). You make up an rs232 lead with an rj11 connector, use a usb to rs232 port adapter and you can set the current on the drives exactly to their rating and then you can tune the PID loop for best performance. My drives are silent now when they run and I don't have any overheating issues, best of all they will error out if there is a problem. Some people have had mixed issues with leadshine, my experience has been very positive, gecko are way too expensive for us in the UK with taxes shipping and duty on the DIY CNC (non money making) side of things.

rbmgf7
Posts: 26
Joined: Sat Apr 01, 2017 5:38 pm

Re: Anyone running UCCNC?

Postby rbmgf7 » Wed Nov 15, 2017 9:54 pm

FYI for Geckodrives:

I started running a G540 at 48V. Ran great for the longest time but suddenly, it started faulting real frequently, especially on startup.

Had no idea what was going on. I caught a thread somewhere where someone was having the same issue. Their solution was to use a lower voltage PSU.

I had a 24V lying around. Swapped it out and the Gecko hasn't faulted since.

rbmgf7
Posts: 26
Joined: Sat Apr 01, 2017 5:38 pm

Re: Anyone running UCCNC?

Postby rbmgf7 » Wed Nov 15, 2017 9:59 pm

Does the UCCNC support THC inputs like Mach3?

I've used ESS and the USS. Been OK. I tried a Masso but it was far from complete.

UCCNC and Dynamotion controllers with software seem like another candidate. Looking for something a little quicker. The M-code pauses are painful when Mach is selecting THC on/off during a cut.

robertspark
Posts: 37
Joined: Mon Jun 12, 2017 6:43 pm

Re: Anyone running UCCNC?

Postby robertspark » Fri Nov 17, 2017 6:09 am

Oh yes, definitely and they offer much much more control..... Quite a bit of time was spent with cncDrive providing the THC features that work seamlessly.

If you have a plasma application and want it running on windows, forget Mach3

there are various macros that can be operated in sync with motion (i.e. there is no hesitation like there is with Mach3 when running a macro or Mcode)

Mach3 only offers M10/M11, Mach4 M62/M63

Uccnc offers:
M10/M11 (same as Mach3 M11/M10 + Mach4 M62/M63 + Linuxcnc M62/M63 ) sometimes referred to as laser output control.

M205/M206 : Turns THC on/off in sync with the motion {same as / more correctly AVC on + off}

M207/M208 : Turns the THC delay on/off in sync with the motion

M209/M210: Turns the THC anti dive on/off in sync with the motion

M211/M212 : Turns the THC anti down on/off in sync with the motion


M213/M214 : Turns the safe probe mode on / off
(this is not really for plasma but for probing, however if you have a G1 rapid move across the table you could enable this and iff for instance your last custs left the cut metal sitting at an angle on the table and the torch was to catch the material it would safely stop the torch as quick as possible and wait for user intervention and reset.

It's actually to prevent a broken probe tip potentially when traversing the table and not in G31 mode.

robertspark
Posts: 37
Joined: Mon Jun 12, 2017 6:43 pm

Re: Anyone running UCCNC?

Postby robertspark » Fri Nov 17, 2017 6:12 am

rbmgf7 wrote:FYI for Geckodrives:

I started running a G540 at 48V. Ran great for the longest time but suddenly, it started faulting real frequently, especially on startup.

Had no idea what was going on. I caught a thread somewhere where someone was having the same issue. Their solution was to use a lower voltage PSU.

I had a 24V lying around. Swapped it out and the Gecko hasn't faulted since.



http://www.geckodrive.com/g540.html

48V is a bit close to the specified maximum rated voltage of 50V IMHO {hence I try to select drives with much higher maximum voltage ratings}


Return to “General Discussion”

Who is online

Users browsing this forum: No registered users and 1 guest