Looking for some help dialing in a Proma SD on a new machine

[xnaron]

Because I cut it out of a relatively small piece I thought it might have moved a bit while cutting it. I watched the video back and I didn't really see a point where it moved but it was hard to tell with sub par camera work.

[robertspark]

I have always found aluminium rough due to the fluidity of the material at temperature with compressed air blasting past the cut edge I suspect.... but it cuts.

[xnaron]

It's messy as well. I will stick to steel for now.

My axbb-e should be here this week. With any luck I will get it installed this weekend and start running UCNC.

[robertspark]

It's messy as well. I will stick to steel for now.

My axbb-e should be here this week. With any luck I will get it installed this weekend and start running UCNC.

I would suggest not using the mach3 XML import but setting the settings by hand in uccnc (too many people use the XML import and then get caught out thinking uccnc is just an upgrade of mach3 ..... there are differences as the motion planner is different etc)

[xnaron]

I didn't even know you could do an import. I am planning on starting from scratch.

[xnaron]

My AXBB-E arrived today. It didn't come with any papers or anything with a license key for UCNC. I am not sure how that works so I emailed them. I'll be tearing down my controller and installing this asap.

[robertspark]

My AXBB-E arrived today. It didn't come with any papers or anything with a license key for UCNC. I am not sure how that works so I emailed them. I'll be tearing down my controller and installing this asap.

email CNCdrive with your serial number of the hardware and email / invoice ref etc and they should email you the file back you place in the uccnc folder

[xnaron]

I decided to just build another controller as I already had most of the components on hand. I designed the layout with the components and cut it on the plasma out of 1/8" sheet aluminum (non 6061). Followed book values and it turned out fantastic. No dross. I used a plasma drill op on all the holes to locate them with the cutter set at 20amps. It still burned all the way through. I was hoping it would dimple.

Included are some pics of how I will layout the components. I need to turn the relay board around as it will be better for wiring. I am missing the 36v supply as it does not come till tomorrow. The slots in the base plate are for routing wires underneath. I am not sure if I will do that but wanted to have the option.

I am glad this worked so well as I can see myself making this type of mounting plate a lot.

No dross!! (Backside)

(Frontside)

[Zukzilla]

How have you managed to stop the proma diving ?

[xnaron]

Well that got out of hand fast. I've been having really good success cutting the panels for the new controller out of 16 gauge. Pretty much dross free with the finecut consumables. I put a kill switch in there to be able to manually disconnect the torch on/off going to the powermax. The empty hole will house the proma sd until I can get a new THC. Then I can just recut the panel to fit whatever I go with. MiniTHC is out of stock as well.

[xnaron]

I am getting some curved corners where they should be a 90 (see arrows in pic). I am pretty sure this is caused by my settings in Mach 3. I Have acceleration set at 40 and I was cutting at 250ipm. I believe that Mach 3 did the best it could but I don't have quick enough acceleration to make the corner at a 90. I am not sure if there is something it sheetcam I can tweak to help this. The other alternative is to bump up the acceleration or lower the speed. I haven't tried tweaking the acceleration. It is set to the factory default mach 3 that Langmuir systems. I have no idea if that is a tweaked or safe setting.

Hand filed the corners

[djreiswig]

Try adjusting the CV setting in Mach. I think it was suggested to me to use 89 degrees, but you'll have to experiment to see what works.
If you slow down it will affect your kerf width and dross.

[xnaron]

Thanks I remember tweaking that on my CNC router. I'll try 89.

It will be interesting to see the differences between Mach 3 and UCNC when I get my new controller going,

[robertspark]

Try adjusting the CV setting in Mach. I think it was suggested to me to use 89 degrees, but you'll have to experiment to see what works.
If you slow down it will affect your kerf width and dross.

Thanks I remember tweaking that on my CNC router. I'll try 89.

It will be interesting to see the differences between Mach 3 and UCNC when I get my new controller going,

The CV setting in Mach3 switches it from constant velocity to exact stop mode (i.e. motion stops at that junction point before accelerating back up to the next gcode co-ordinates.

Mill + plasma are different ....

there is a manual (pamphlet?) explaining some of the settings that were never covered in the Mach3 manuals (a big failing of Mach3..... manuals and information....)
https://www.machsupport.com/wp-content/ ... ngs_v2.pdf


40 "/s/s and 250 ipm = minimum corner radius of 0.43" (without slowing down).

really you can allow for the junctions with a little dross and overburn so feedrate can drop to about 60% of the linear feedrate (you DONT want to turn off CV which is what setting " Stop CV on angles >" does (IMO / YMMV)

at 60% of 250ipm = 150ipm
therefore allowable minimum radius would become 0.156"
https://www.khanacademy.org/science/phy ... celeration (see example 1 if you are interested in the simple math)

try to change the CV Distance Tolerance to something like 0.15 if you want minimum dross, or if you want a tighter corner say 0.1" (2.54mm)

note this presumes that you ARE running your machine in inches.... scale by 25.4 if you are actually running in mm or the machine will try to create inside radii of 0.1mm which on a plasma is pointless considering the kerf width and you've get a lot of overburn and dross. this is something that you will come across with UCCNC with the most important sections of the manual and setup being G64 / the Corner Error Max setting (which most people including me did not realise / understand its importance and glazed over the uccnc user manual when setting things up).

These settings below allow for greater control with UCCNC than Mach3 and also ensure that the motion controller obeys the limiting settings of the planner (you will probably get higher acceleration with UCCNC as I'm told that Mach3 can violate the maximum acceleration settings on occassion which leads to lost steps which is why you tone down the acceleration in Mach3 below what is used in uccnc..... or that seems to be the common finding between those that convert from Mach3 to uccnc anyway (judge for yourself by retesting your machine stall / lost steps points with velocity and acceleration settings))

[djreiswig]

Thanks robertspark. I'll have to play with the CV dist tolerance. Never knew what it did.

[xnaron]

Thanks for the excellent explanation. I am working through it all. Using the linked equation in example 1 I calculate that I would need to set acceleration to 115 inch/s/s to get 0.15 radius at 250ipm. I have not done a test on my machine to see what is the max acceleration before losing steps. As you said I could drop the feedrate to 60% to get that as well. Does the powermax plasma amps scale linearly? Ie: if I was cutting at 45 amps and 250 ipm would it be 60% of the amps for 60% of the feedrate?

Thanks,
Brendin

[robertspark]

I think you may be misunderstanding the 60% drop in feedrate. (this is also a bit key to plasma cutting and thc settings)

you don't change the amperage or feedrate from the linear feedrate all you do is set the parameters G64 so that the planner adjusts the feedrate

[xnaron]

I think you may be misunderstanding the 60% drop in feedrate. (this is also a bit key to plasma cutting and thc settings)

you don't change the amperage or feedrate from the linear feedrate all you do is set the parameters G64 so that the planner adjusts the feedrate

Ok I understand now. Thanks. I am waiting on the last power supply to arrive today and I will start wiring the new UCCNC controller. I am looking forward to trying it.

[robertspark]

sorry split posts.... needed to change from a phone to a keyboard....

It took me a while to figure out the importance of G64 and being able to set and control its parameters which in turn creates the part you want.

G64 is not adjustable on the fly in Mach3/Mach4 as it is in UCCNC, LinuxCNC

to start with the basics...

Exact stop is easy to understand (G61)...

Code: Select all

G92 X0 Y0
G61
G1 X100 F250
G1 Y100
G1 X0
G1 Y0

will move in a square, and at each node the machine will decelerate to a stop before accelerating back up to the feedrate and off to the next node / co-ordinate location.

G64 is constant velocity mode, and the one that takes a little more thought....
And the bit that most people don't get (I never got it for ages.... maybe I'm just thick!)

remember that most machines are 2 axis linear motion so to draw any shape one axis has to slow down for the other to speed up so if you move in a square in constant velocity at some point one of the axis needs to slow down (at the defined acceleration) and the other needs to begin speeding up (at the defined acceleration)
So we now have the blended velocity which is the feedrate of one axis as it slows down and the other as it speeds up.

The problem is as one of the axis is slowing down and the other is speeding up the machine is moving away from the defined end co-ordinates of the move and this will form a radius as those two axis change their velocity but maintain the blended velocity.

In steps the CV parameter (in Mach3 it is the "CV Distance Tolerance" and in UCCNC it is the "Corner Error Max" and in LinuxCNC it is paramater "P" (motion blending tolerance) https://linuxcnc.org/docs/2.6/html/gcod ... ml#sec:G64

In UCCNC and linuxCNC you can set the tolerance from within your post processor so that they can be specific to what you are trying to cut (material thickness / feedrate) and not a one time setting which is what it is in Mach3 (or Mach 4 (i think)) which means you have to change it manually

If the parameter is set very large then it has no effect on lowering the feedrate so the machine will maintain CONSTANT VELOCITY..... all through the move...... but if you add in a G64 tolerance parameter what that does is it forces the planner to slow the velocity down so that when the planner plans the junctions between the sections of the gcode so then it comes to deciding how much you want to allow the gcode to slow down.

the 60% comes from the allowable feedrate drop for small arcs and holes and circles where you lower the feedrate in order to minimise the cut edge bevel at the cost of a bit of increased dross.

Don't change the feedrate at the corners, allow the machine to lower the feedrate automatically by forcing it to track the tolerance parameter you set.

______________________________________

With regards to the THC, some motion controller software has a torch height control parameter which ignores THCDN if the feedrate drops below a certain percentage..... say the linear feedrate is 250ipm, if you set this THC setting at 80% of feedrate, as the machine accelerates up to 200ipm and decelerates below ipm the motion controller will ignore THC down signals.

the same at junctions.... back to the same square gcode above....

if you set the CV corner tolerance to say 0.2" (5.08mm radius [i.e. units before and after the junction])
you will now force the machine to lower its feedrate so that it can achieve the tolerance parameter you required.

say the acceleration is 40i/s/s... so the feedrate would have to drop from 250 ipm to 170ipm in order to achieve the corner tolerance you have set.

if you use a code snippet to change the feedrate to say 170ipm 0.2" before and change it to 250ipm 0.2" after the corner the THC will not be disabled / it will not ignore the THCDN signal because you've just changed the feedrate it sees from 250ipm to 170ipm..... where as if you left the linear feedrate alone and set the ignore THC dn below 80% feedrate, when the feedrate dropped below 200ipm the torch would not dive as the voltage increased and when the machine accelerates back up above 200ipm the THC would automatically be re-enabled.


In mach3 on the plasma screen its shown as the "THC Min Speed" setting, and in UCCNC it's called the "Anti-Dive %" which is the same a percentage below the programmed feedrate where the THC DN/UP signals are ignored automatically.

I am sure LinuxCNC has a similar setting too (but I don't have a screenset to hand to screenshot)

[xnaron]

Passed the initial smoke test. Still need to wire all the connectors.

[acourtjester]

I see you are using the crimp connectors on your wiring, they work great for the smaller connections on those screw connectors:Yay

[xnaron]

Yes! They are awesome.

[Rodw]

A very interesting discussion here. I was rereading the linuxcnc docs the other day and found that the ini file allows you greater control over the trajectory planner's behaviour.
http://linuxcnc.org/docs/2.8/html/confi ... aj_section

It occurred to me the other day that as users we blindly accept the default values here. But hang on! They will have been set for use on a milling machine. Plasma is different as Robert says. I think some serious experimentation is required to obtain plasma specific optimum values.

at 60% of 250ipm = 150ipm
therefore allowable minimum radius would become 0.156"
https://www.khanacademy.org/science/phy ... celeration (see example 1 if you are interested in the simple math)

I've been working through the maths here right now and this is the incorrect approach. An engineer I know pointed out to me that you also have to account for the difference between centripetal acceleration and linear (tangential) acceleration. With a bit of research I found he was correct. Radial acceleration is in radians/sec^2 but our machines are designed with acceleration of metres/sec^2.

So I came up with an exam question to solve for.

A tool on a CNC machine is travelling at 10.24 metres per minute (0.17067 metres per second) can accelerate at 5 metres per second.
What is the minimum arc radius it can follow at that velocity?

A mistake I always make here is forgetting to change the velocity to SI units (metres/second) so I included it in the question for convenience.
To solve this, you end up with two formulas for the radius to solve for by substitution
As of yesterday with the help of another Linuxcnc stalwart who just happens to be an engineering professor, the unconfirmed (for me) answer is 0.7mm
So any other submissions will be accepted by the examination board as I really want to understand this

Hypertherm talks about centrepetal limiting where the velocity is constrained based on the physics. Reducing the velocity by 60% I suspect is a simple solution that can be applied on any machine. But what I want to be able to do is calculate this velocity override dynamically based on the arc radius in real time. So basically develop some algorithm that changes this override and possibly even the motion path based on the arc radius within the motion controller without using g code at all

[xnaron]

The final push on the controller and the last cut the old controller will make which is the support brackets for the new controller.

[robertspark]

very nice