sheetcam anti dive how to

[4130metalworks]

Hi, i am trying to find information on the anti dive feature in sheetcam. How does it work and what is the percentage representing? I already have the path rules set to turn thc on and off on corners and circles but was wondering if this was another way of doing this
thanks for all help

[sheetcamCS2]

You mention that you're already turning the THC Off and On on corners and circles. That IS the Sheetcam implementation of anti-dive.

The triggers for 'On all corners' rule is a distance before and after the corner, qualified by the 'tighter than' degree of the corner angle, or in other words the minimum degrees to define a corner needing the rule. The 'feed rate %' is a parameter to OPTIONALLY ALSO or EITHER change the feed rate during the trigger condition. The feedrate could help mitigate dross on the bottom side of the cut.

You can also consider the rule 'Before end' for THC Off action to implement anti-dive while the torch decelerates at the end of the cut, and depending on your THC On delay settings, consider rule 'On start' for THC On action to do the same near the end of acceleration.

The distance you use in the rules for the period that the THC is Off depends on your controller's XY acceleration configuration. Usually, a distance of 5mm into and 5mm out of the corner, or from start or before stop, is sufficient.

[adbuch]

Lou - thanks for that great explanation and welcome to the forum!!
David

[Dirtmotor]

Good Info thanks , glad you joined .

[4130metalworks]

thanks Lou, so just leave the anti dive percent at zero in the jet tool and keep playing with path rules

[sheetcamCS2]

@4130... well, not exactly. There is no 'anti-dive percent'. There is however a 'feed rate %'. If you are seeing an 'anti-dive percent' in Sheetcam, then you are using a plugin that I'm not familiar with, or a post processor adding a DefineCustomToolParam() to the PlasmaTool.

If we're strictly talking about the concept of an anti-dive implementation in gcode that stock Sheetcam can provide while cutting a sharp corner, then here is an example...

In this example, the 'programmed' feed rate is unchanged, aka 100%. Although, for any CNC to negotiate such a corner, the XY motion will actually decelerate, change course (direction), and accelerate; the CNC controller handles this automatically. If you want to change the programmed feed rate, then use a percentage other than 100%, but there will still be some CNC controller managed decel/accel conducted.

All of this applies to other rules in the 'rule' drop down list. You should explore them, then examine the gcode produced during post processing. This is a very powerful feature to affect some anti-dive measures via gcode. Know that some rules can be written to contradict others, so I recommend that you explore them individually first. If combining rules, the order of precedence can get complicated.

[sheetcamCS2]

@1430... I may understand your point of view better now, I'm sorry about the confusion. I just searched the Sheetcam library of post processors for 'anti dive' and found hits in two Masso .scposts. Couple that with your mention of "...Masso is going to release it one day", and now I suspect you are using one of the two Masso .scpost ? If that is correct, then you have to consult the Masso controller manual as to the use of that additional PlasmaTool parameter. That parameter is not stock Sheetcam, but as you can see, Sheetcam is designed to allow for user defined custom parameters to be added to tool definitions. Based on what I see in the .scpost, it's used on the Masso G200 command, 'A' word value, as a percentage value as you noted, in OnToolChange() function, so anytime the tool is changed in a subsequent Jet Operation.

I hope this helps.

[4130metalworks]

Great detective work Lou, i didn’t realise there was a difference with the masso sheetcam and others
Masso has anti dive on the back burner so if its their post processor it’ll most likely never happen

I will keep playing and learning about path rules for now

[tcaudle]

Anti-dive is a cath all term without a lot of regard as to WHAT it mens.

Basically a plasma torch cuts metal with voltage and current . Current stays constant (or should) so the "resistance" of the arc and the metal define the resistance. As resistance varies voltage varies with it so if you measure voltage its SHOULD predict resistance. Since the Arc GAP is typically the major resistance factor you can use it to measure "height". Works great asl long as the other variables are kept constant.
What are the other variables? well, the metal thickness , the work clamp connection and (Ding Ding) the feedrate. When motion slows the voltage goes UP causing the torch to DIVE to try and "fix" it .

The more accurate your table tracks the more slowdowns it faces . It means the toolpath cant be deviated from so the controller "drives" the course and slows down/speeds up a lot to stay on track.

The simplest form of anti dive is to try and look at the shapes you cut and predict when a slowdown will occur.
Sheetcam has built in CUT RULES that analyse the tool path and "trigger" a rule to cause an ACTION: That can be simply an OFF of the THC if it has a G or M command that will do that IN MOTION. If your in/off causes a pause in motion then its not suited for active anti dive. So controllers allow that, some do not.

So you tell it on corners "less than X Deg" to turn off the THC so it does not dive. Cut rule in SHeetCAM. Another useful one is the EOC (end of cut that turns off the THC some fixed distance before the end of cut and that ugly voltage spike of approaching the beginning cut (lead in) ant he piece falling out causes the torch dive at the end.

You can also look at t an upcoming cut and turn off the THC of it too short . SheetCAM has a variable (internally)( called EnityLenght. It tesl you how long the NEXT cut is before you make it!

A more advanced form of anti dive monitors the ACTUAL feedrate in REAL TIME and when the motion slows for ANY reason it turns off the THC . You have to have a way to measure the real time speed and a way to rapidly turn off and on the THC as it cuts. Its Called VAD (Velocity Anti Dive) With it you don't need Cut rules (except for the End of CUt). The torch can drive the tool ptahs , slow down and speed up as it needs to (provided you have a good trajectory planner in the motion control) and stop diving on corners , turns, angles or any details that cause the torch tot slow . The percentage (trigger level) of slow down needs ot be adjustable

Its simply not possible to do with most Windows based controllers since there is a dealt between reeding and executing the G-code and it actually being sent to the hardware. The commanded velocity is not useful just the ACTAUL speed.

Dirty little secret is the term "Automatic Torch Height " cam mean a lot of things and not all have the features you might want.

[Dirtmotor]

Here are some of my path rules , how do I add turn off thc ? There are a lot of speed changes , My diving problems are mostly on 16 guage ?

sheet cam.png (78.45 KiB) Viewed 2166 times

sheet cam.png (78.45 KiB) Viewed 2166 times

[sheetcamCS2]

attached is a sample toolset implementing THC OFF/ON control as an anti-dive measure using Sheetcam rules.
The code snippets that control the THC in this use case must use continuous motion gcode. Some controllers require laser mode ($32=1) for this type of continuous motion when changing 'S' word (spindle speed or laser power). As such, some plasma controllers use the 'S' word to control THC OFF/ON state for the same continuous motion effect.

Without the ability to manage THC OFF/ON state under continuous motion, as @tcaudle explained, the controller will decel XY and stop in order to issue a THC gcode synchronous with the XY position; translation, that's meaningless to attempt to manage THC for anti-dive in this condition.

So you must know your CNC controller and its ability to issue THC control (gcode) while maintaining continuous motion in order to manage anti-dive with Path rules. And you must know your THC OFF/ON gcode commands and apply them to the code snippets in the example given.

I hope this helps.

THC sample rule set.zip

(687 Bytes) Downloaded 18 times

THC sample rule set.zip

(687 Bytes) Downloaded 18 times

[Dirtmotor]

Could not open your file

[tcaudle]

Could not open your file

It should download (or at least prompt you to Save or run) save it then open the zip locally and its a toolset. Move it to the directory you have your toolsets in and then sue the Load Toolset option in SHeetCAM. The tool-set holds cut rules and any Code snips

You have a choice of running a cut rule on each operation OR you can define a Path Rule and set the cut tulle to be Used on every operation (automatically )

If you can find an in-motion THC ON/OFF then you have options to do things outside of cut rules .

16 ga moves a lot faster and things happen a lot quicker so its more sensitive to THC issues.

[tcaudle]

All those path rules do is slow down feedrates. The do nothing to support anti-dive of any kind.
When you slow down feed rates the torch dives (THC operation 101)

[sheetcamCS2]

@tcaudle- I appreciate the input and I agree with all of your prior points. However, if you are referring to the 'THC sample rule set' that I posted, those code snippets for THC OFF/ON do not change feedrate, nor does the rule feedrate %.

The gcode in the code snippets change 'S' spindle speed, also known as laser power when $32=1 (laser mode) controller config on some controllers. Spindle speed is usually a PWM (pulse width modulated) output, which can also be used to control some THC OFF/ON on some units. The advantage of using 'S' word to do this is that its conducted by the controller with continuous motion when the controller is in 'laser mode', IF motion is also specified on the same line, hence the G91 (relative dist mode), then G1 X0 (essentially no motion), then Snnn, where nnn values dictate OFF or ON thresholds of the PWM signal. And then the second line puts the controller back in absolute dist. mode, G90.

I actually use this code on my CNC table for THC OFF/ON control.

[Dirtmotor]

All those path rules do is slow down feedrates. The do nothing to support anti-dive of any kind.
When you slow down feed rates the torch dives (THC operation 101)

Yes I understand that. My question is how to add the THC Off to rules , Thanks

[sheetcamCS2]

@dirtmotor- did you eventually get the sample rules file loaded ? And does the example with code snippets explain how you add gcode to manage the THC OFF/ON ?

[Dirtmotor]

No , dont seem to have anyplace that I can open them .

[sheetcamCS2]

try this...

[Dirtmotor]

Thank you . That opened up for me looks good . I will play with the rules this weekend .

[tcaudle]

@tcaudle- I appreciate the input and I agree with all of your prior points. However, if you are referring to the 'THC sample rule set' that I posted, those code snippets for THC OFF/ON do not change feedrate, nor does the rule feedrate %.

The gcode in the code snippets change 'S' spindle speed, also known as laser power when $32=1 (laser mode) controller config on some controllers. Spindle speed is usually a PWM (pulse width modulated) output, which can also be used to control some THC OFF/ON on some units. The advantage of using 'S' word to do this is that its conducted by the controller with continuous motion when the controller is in 'laser mode', IF motion is also specified on the same line, hence the G91 (relative dist mode), then G1 X0 (essentially no motion), then Snnn, where nnn values dictate OFF or ON thresholds of the PWM signal. And then the second line puts the controller back in absolute dist. mode, G90.

I actually use this code on my CNC table for THC OFF/ON control.

Its totally dependant on HOW the THC is enabled/disabled or even if it can be.
If it can use a simple output in Linuxcnc you have M codes that use IN-Moiton (synchronized) . M67 with the E and Q to point to the correct output is synchronized with motion . For example with CommandCNC (based on Linuxcnc) the POST calls M67 E0 Q10 to turn the DTHC off and M67 E0 Q20 to turn it on while its moving. To do it immediate you use an M68 but that executes as a separate line and will pause motion if used in the wrong place. Code snips for the DTHC use those codes to control on/off of the DTHC

Its up to the controller and its dialect of G-code and also HOW the THC can be turned off and on remotely. Not all allow that .

The "S" command can be used for other things besides spindle speed. Its up to how the g-code parser in the mtion control reads it. We have used it for years to set various THC parameters based on a three or 4 digit number. First number tells it WHAT parameter while the next two or three digits is the value . Thus a number like 4135 can mean set the voltage preset at 135vols

The beauty of SheetCAM is its LUA POST language and how the POST can change the way SheetCAM presents options and tool parameters.

[adbuch]

Great discussion here!! Very informative about gcode implementation for various thc units.
Thanks,
David