my newest Sheetcam head scratcher.

[Deezl Smoke]

This sort of goes along with my prior path rules thread, but new and a bit different. I have the rules thing almost nailed now thanks to the members here.
However,.... this morning I am cutting a bunch of .25" A36 mild to brake for some building down spout guards. Need to cut 12 holes .6875" diameter in each piece.
Cut a few test strips to calibrate the press brake. For the life of me, I could not figure out why dthc would come on and stay on in the small circles when the path rule for small circles was correct. Kept trying different things, restarting the computer, reloading the rule, etc. I have no idea why, but I noticed I was using perpendicular lead in on the circles. All I did was change that to arc, and issue solved.WTH? I use perpendicular lead in for the outside offset.
Must be something to do with the straight line not identifying the circle as a circle, but a shape? Dunno. Now I know to watch for that, on my old linux machine anyway.
Once I made that correction,...I am so happy with how the cutting is going. May try to get some video this afternoon as the cutting gets closer to finishing.

[adbuch]

This sort of goes along with my prior path rules thread, but new and a bit different. I have the rules thing almost nailed now thanks to the members here.
However,.... this morning I am cutting a bunch of .25" A36 mild to brake for some building down spout guards. Need to cut 12 holes .6875" diameter in each piece.
Cut a few test strips to calibrate the press brake. For the life of me, I could not figure out why dthc would come on and stay on in the small circles when the path rule for small circles was correct. Kept trying different things, restarting the computer, reloading the rule, etc. I have no idea why, but I noticed I was using perpendicular lead in on the circles. All I did was change that to arc, and issue solved.WTH? I use perpendicular lead in for the outside offset.
Must be something to do with the straight line not identifying the circle as a circle, but a shape? Dunno. Now I know to watch for that, on my old linux machine anyway.
Once I made that correction,...I am so happy with how the cutting is going. May try to get some video this afternoon as the cutting gets closer to finishing.

[sheetcamCS2]

@deezl, I don't believe the path rule is supposed to behave differently based on leadin style. I just tried a simple test case and don't find the different behavior, in v7.0.21 or 7.1.40. If you'd like to send me a support.zip file I can have a look. see instructions here- https://forum.sheetcam.com/t/creating-a ... file/8078/
thanks.

[Deezl Smoke]

@deezl, I don't believe the path rule is supposed to behave differently based on leadin style. I just tried a simple test case and don't find the different behavior, in v7.0.21 or 7.1.40. If you'd like to send me a support.zip file I can have a look. see instructions here- https://forum.sheetcam.com/t/creating-a ... file/8078/
thanks.

I'm hoping to finish this job, then use a piece of scrap and test my theory. I'll try to video it first, then if it does make a difference, I'll send a support file.
On another note, below the lead in lead out options, there is a "start at center of circles smaller than____" I have that set to 2". I don't know if that has anything to do with it or not.

[tcaudle]

Ill throw this out there: DO NOT use any CUt RULES from SHeetCAM with CommandCNC EXCEPT EOC (End of cut. why:
1. COmmandCNC and the custom POSTS for SheetCAM have CUt rules built in , It has parameters in the toolset and using SheetCAM internal variables to control the cutting. Setting a cut tule can conflict with the internal tules and cause unwanted actions. Example" the rule to turn off the THC on circles smaller than X is already handled in a tllset parameter called |Min Cut Length for DTHC: it defaults to 1" and keeps the DTHC for ever turning on at the beginning versus try to turn it off. The DTHC doe NOT automatically turn on when you fie the torch. It FIRST looks at the length of the upcoming cut (thanks to a variable in SheetCAM call "entityLenght" and if it's GREATER than the Min Cut Length you have set, it lets the sequence occur. The "sequence is" Fire the torch. Pause until you get ARC OK. Paise for Pierce Delay, Move from Pierce Height to Cut height and THEN enable DTHC AFTER the DTHC Delay (another parameter you set)

So if you inject other rules in that sequence it disrupts the flow and can result tin the wrong action,

The BEST way to cut smaller holes because they need to be done at slower feedrates and with the DTHC off is to put them in a stepper Layer and a separte OPERATION ans either set the "Min Cut L:enght : to a number above the Circumferece of the biggest hole Plus leadin/ot OR simple use the "Disable DTHC this Operation" check box.

The DTHC5 is a lot more advanced than most THC's and coupled with the logic we put in the POST for SheetCAM (thnaks to its open programming interfae)

Also the Real Time feedback in LinuxCNC and CommandCNC gives functions like "Cornerr Slowdown and Anti-dive a way to do those functions without complex rules. The trajectory Planner in LinuxCNC tracks the toolpath tightly and slows down automatically to match what the mechanics can do. As a result it slows down on tight turns and comers at a smoother rate and that tells the DTHC to turn off until speeds get back to normal and presenting diving on details and corners. No RULES needed and they will conflict and nullify the VAD operation.

[Deezl Smoke]

Ill throw this out there: DO NOT use any CUt RULES from SHeetCAM with CommandCNC EXCEPT EOC (End of cut. why:
1. COmmandCNC and the custom POSTS for SheetCAM have CUt rules built in , It has parameters in the toolset and using SheetCAM internal variables to control the cutting. Setting a cut tule can conflict with the internal tules and cause unwanted actions. Example" the rule to turn off the THC on circles smaller than X is already handled in a tllset parameter called |Min Cut Length for DTHC: it defaults to 1" and keeps the DTHC for ever turning on at the beginning versus try to turn it off. The DTHC doe NOT automatically turn on when you fie the torch. It FIRST looks at the length of the upcoming cut (thanks to a variable in SheetCAM call "entityLenght" and if it's GREATER than the Min Cut Length you have set, it lets the sequence occur. The "sequence is" Fire the torch. Pause until you get ARC OK. Paise for Pierce Delay, Move from Pierce Height to Cut height and THEN enable DTHC AFTER the DTHC Delay (another parameter you set)

So if you inject other rules in that sequence it disrupts the flow and can result tin the wrong action,

The BEST way to cut smaller holes because they need to be done at slower feedrates and with the DTHC off is to put them in a stepper Layer and a separte OPERATION ans either set the "Min Cut L:enght : to a number above the Circumferece of the biggest hole Plus leadin/ot OR simple use the "Disable DTHC this Operation" check box.

The DTHC5 is a lot more advanced than most THC's and coupled with the logic we put in the POST for SheetCAM (thnaks to its open programming interfae)

Also the Real Time feedback in LinuxCNC and CommandCNC gives functions like "Cornerr Slowdown and Anti-dive a way to do those functions without complex rules. The trajectory Planner in LinuxCNC tracks the toolpath tightly and slows down automatically to match what the mechanics can do. As a result it slows down on tight turns and comers at a smoother rate and that tells the DTHC to turn off until speeds get back to normal and presenting diving on details and corners. No RULES needed and they will conflict and nullify the VAD operation.

Your first paragraph helped me a lot. Now I have an idea how the dthc and min length parameters function,...kinda.
But I have tried no rules and I end up with bad corners in heavy plate when I can not put a radius on them. I need to slow the torch at those corners. When I use the path rule to slow it to 70% and turn off thc, then turn on thc once past the corner, it works awesome and makes much nicer corners.
But I do recall you saying no rules a few times in the past. I just can't seem to get certain results without them. Now, when I took the whole control cabinet to Arclight for inspection and repair if needed after the lightning strike, they too mentioned just as yourself, that I had some rules conflicting with others. So they cleaned them up.
I still want to do a test cut for fun and learning on a scrap piece using the perpendicular vs. arc on small circles. Might show a glitch in my system that needs addressed otherwise.

[adbuch]

I still want to do a test cut for fun and learning on a scrap piece using the perpendicular vs. arc on small circles. Might show a glitch in my system that needs addressed otherwise.

I will look forward to seeing your results on that one with the different lead-ins.
David

[tcaudle]

If you need the machine to slow down more on corner then setup a different CONFIG tune the Acceleration on X and Y (not Z) down to 15 IPS/sec That will cause the trajectory engine to automatically slow down the motion as it approaches the corner and turns off the DTHC.

Also look in the POST and see were your Tracking and tolerances are set . The tighter that is the sharper the tunr and the better the CVAD will work .

If you decide to continue to use the cut rules than turn off VAD and let tthe run disable the DTHC. I wont gurantee it will work perfect but you dont want dueling rules .

The other thing its to check your CommandCNC release number. It heeds t o be at least 1.2 or higher. VAD stops working if you use the velocity slider to manually slow it down on the older versions. Updates are free and they are on the SUPPORT/DOWNLOADS section of the website,

Consider the trajectory engine is like a driver on a winding road trying to move as fast as they can but not vary out of their lane, It looks ahead and decides to slow down enough to safely make a turn based on the ability of the vehicle (Machien) YOu tell it waht the machine can do and how fast it can take a corner by definieng how quickly it can accelerate/decelerate.
There are times when you want very tight toolpath tracking and others where if you are cutting something that is "ragged" (like some artwork files you see) you want the motion to be smoother and allow the motion to bot follow the toolpath as tight . YOu have to change that on the preamble of the post so having more than one copy of a POST with some different parameters for different types of cutting might be in order.

it tough to cut a square corner (inside cut) with a round tool and plasma flame is round. There will always be a small radius .

[Deezl Smoke]

If you need the machine to slow down more on corner then setup a different CONFIG tune the Acceleration on X and Y (not Z) down to 15 IPS/sec That will cause the trajectory engine to automatically slow down the motion as it approaches the corner and turns off the DTHC.

Also look in the POST and see were your Tracking and tolerances are set . The tighter that is the sharper the tunr and the better the CVAD will work .

If you decide to continue to use the cut rules than turn off VAD and let tthe run disable the DTHC. I wont gurantee it will work perfect but you dont want dueling rules .

The other thing its to check your CommandCNC release number. It heeds t o be at least 1.2 or higher. VAD stops working if you use the velocity slider to manually slow it down on the older versions. Updates are free and they are on the SUPPORT/DOWNLOADS section of the website,

Consider the trajectory engine is like a driver on a winding road trying to move as fast as they can but not vary out of their lane, It looks ahead and decides to slow down enough to safely make a turn based on the ability of the vehicle (Machien) YOu tell it waht the machine can do and how fast it can take a corner by definieng how quickly it can accelerate/decelerate.
There are times when you want very tight toolpath tracking and others where if you are cutting something that is "ragged" (like some artwork files you see) you want the motion to be smoother and allow the motion to bot follow the toolpath as tight . YOu have to change that on the preamble of the post so having more than one copy of a POST with some different parameters for different types of cutting might be in order.

it tough to cut a square corner (inside cut) with a round tool and plasma flame is round. There will always be a small radius .

THAT !! is a lot for this old man to digest. Some of that is over my head, but as I have been finding out lately, the more I can learn of how this machine works, the better I get at real time trouble shooting and the happier I am with it's performance. So I'm going to copy paste and print that reply so I can take it to the shop and find some of the settings.
I don't know what VAD is yet, but my torch uses digital thc, not ohmic just for reference.
Here's an older picture of one of the screens. It shows version 1.2 firmware.
The only sliders I ever touch are in the lower left corner. When I need to manually cut off a rem or clean up a plate, I lower the jog speed to the ipm rate etc.
And for some reason, since the lightning strike, I have to hit the reset on the "feed override" slider 9 of 10 times I start the machine up. I can close the program and re-open without hitting reset, but after computer shut down, it's a crap shoot whether the override will be at 95% or 100.

[tcaudle]

VAD is velocity Anti-Dive. Its that setting in your picture upper right input box and defaults to 85%. So what that means is:
when the combined VELOCITY of XY drops to less than 85% of the NORMAL feedrates passed form the G-code (IPM ) it shuts the DTHC Off. When it comes back to 100% it turns back on, The Z does not move during a cut if the DTHC does not move it.
Note on the screen you have VELOCITY ANTI DIVE checked ON so its doing that

I don't know what VAD is yet, but my torch uses digital thc, not ohmic just for reference.

How you do touch-off has no bearing on the actions of the DTHC. Touch-Off is a process done entirely outside the actual DTHC actions,. The DTHC does not even come on until after the sequence of events I listed in the prior post.

Evn on system that use Ohmic , we still suggest the floating torch holder and the mechanical switch as a backup

The whole touch off is controlled from a stored procedure ("macro" to the old MACH crowd) , and does not need the DTHC to run,

Kinda like in an airplane, ignoring a lot of the readouts and settings can cause some bad flights and poor landings.
I know its tedious and boring but the Bladerunner for CommandCNC and the DTHC IV Setup and Testing manual have most of this (and more) in them.

Another suggestion if you still get diving after lowering the Acceleration on X and Y, is to INCREASE the VAD to 90 (Never go to 100 or it just keeps the DTHC off all of the time)

[Deezl Smoke]

Oh right, anti-dive. It's that V in front that doesn't seem to register in my brain.
That picture is older and shows the tip saver still checked. I turned that off per your recommendation and it works so much better now. I'll try to get a few updated pics when I get a chance. I also slowed the Z response like you mentioned, and that too seems to help. But I have noticed that the more dross/slag I get chipped off and burned off of the table slats, the less pogoing the Z does when the torch crosses a slat.

[TJS]

I have two configurations, one for thinner material and one called "Thick Material" where the settings are slowed down as per Tom's suggestions. I was getting torch hop/oscillation on thicker material. I use the "Thick Material" configuration on anything around .25" and above. I have two desktop ICONs, one just called "Plasma" and another called "Thick Material". Also for thicker material I usually do not use the DTHC. I just check box it Off in my sheetcam plan. However unless your table slats are real uneven, YMMV.

[adbuch]

I have two configurations, one for thinner material and one called "Thick Material" where the settings are slowed down as per Tom's suggestions. I was getting torch hop/oscillation on thicker material. I use the "Thick Material" configuration on anything around .25" and above. I have two desktop ICONs, one just called "Plasma" and another called "Thick Material". Also for thicker material I usually do not use the DTHC. I just check box it Off in my sheetcam plan. However unless your table slats are real uneven, YMMV.

[tcaudle]

hat picture is older and shows the tip saver still checked. I turned that off per your recommendation and it works so much better now.

Hopefully you are not confusing TIP SAVER with VELOCITY ANTI-DIVE! Tip saver is an OLD simple voltage based anti dive that locks Z if the voltage suddenly spikes . Problem is if that spike is caused from the torch being too high it locks forever

The V in VAD stands for VELOCITY (aka Feedratel; aka Cut Speed) The motion control has a constant report of the actual Velocity of the cut and compares that ot he requested feedrate on the code and uses that to control the DTHC. It wont lock like tip saver does as long as motion returns to full feedrates .

Do NOT turn off VAD unless yew want NO antidive,

TIP SAVER is no longer even an option on the newest CommandCNC .

[Deezl Smoke]

hat picture is older and shows the tip saver still checked. I turned that off per your recommendation and it works so much better now.

Hopefully you are not confusing TIP SAVER with VELOCITY ANTI-DIVE! Tip saver is an OLD simple voltage based anti dive that locks Z if the voltage suddenly spikes . Problem is if that spike is caused from the torch being too high it locks forever

The V in VAD stands for VELOCITY (aka Feedratel; aka Cut Speed) The motion control has a constant report of the actual Velocity of the cut and compares that ot he requested feedrate on the code and uses that to control the DTHC. It wont lock like tip saver does as long as motion returns to full feedrates .

Do NOT turn off VAD unless yew want NO antidive,

TIP SAVER is no longer even an option on the newest CommandCNC .

Nope, not confusing the two. But shortly ago you helped explain that the tip saver was freezing my Z axis and causing several issues I was having. You mentioned to disable it. I did, and it worked great to do so. Thank you for that.

[Deezl Smoke]

I have two configurations, one for thinner material and one called "Thick Material" where the settings are slowed down as per Tom's suggestions. I was getting torch hop/oscillation on thicker material. I use the "Thick Material" configuration on anything around .25" and above. I have two desktop ICONs, one just called "Plasma" and another called "Thick Material". Also for thicker material I usually do not use the DTHC. I just check box it Off in my sheetcam plan. However unless your table slats are real uneven, YMMV.

I tried the no thc, but many of my cuts can be 6 to 10 feet long Y, then 5 feet X. There's just enough benefit to leave it on. IMO.
How did you set up two icons? That's a cool idea. I'm just not sure how to do that with a single program.

[TJS]

I have two configurations, one for thinner material and one called "Thick Material" where the settings are slowed down as per Tom's suggestions. I was getting torch hop/oscillation on thicker material. I use the "Thick Material" configuration on anything around .25" and above. I have two desktop ICONs, one just called "Plasma" and another called "Thick Material". Also for thicker material I usually do not use the DTHC. I just check box it Off in my sheetcam plan. However unless your table slats are real uneven, YMMV.

I tried the no thc, but many of my cuts can be 6 to 10 feet long Y, then 5 feet X. There's just enough benefit to leave it on. IMO.
How did you set up two icons? That's a cool idea. I'm just not sure how to do that with a single program.

I did it a while ago. I am sure Tom C will be here to tell you. Don't take my word verbatim how to do it. What I did was copy my original configuration as to lets say Configuration2. Then go into configuration 2 and make your changes to slow everything down for thick material. Save it. Save it to the desktop and right click rename "Thick Material" or whatever you want it to be labeled as.

[tcaudle]

The CONFIGURATOR app on the desktop lets you do all sorts of things . They are like the Profiles in MACH. You can have as many as you want.
use this icon

ConfiguratorIcon.png (13.04 KiB) Viewed 1410 times

ConfiguratorIcon.png (13.04 KiB) Viewed 1410 times

You can also access the Configuration tool from a running config using the top eft menu and the MACHINE option.

be aware that the CONFIGURATOR lets you add . delete copy and make read-only CONFIGS and your running config MAY not be the one that defaults when you open the tool

ConfigMain.png (73.52 KiB) Viewed 1410 times

ConfigMain.png (73.52 KiB) Viewed 1410 times

Note at the top you have a FILE. OPEN , SAVE and HELP buttons Thsoe let you OPEN different CONFIGS make any changes ans SAVE them. The FILE button lets you create a NEW Config based on just a DEFAULT Config OR you can COPY (clone) an exiting CONFIG and rename it. Anytime you create a new CONFIG it adds that named icon to your desktop
Best to name it something that identifies it Each CONFIG is totally separte from the motor tuning to the INPUTS s

If you want a more in-depth tutorial get the (dreaded) CCNC-BladeRunner-REV2FullManual.pdf to page 58 and it show you have ot make configs and copy exiting ones . That way you can try stuff and you always have your ground zero CONFIG .

Having multiple CONFIGS for cutting different types and gauges of metal (well, 1/4" and below, then above that for thick stuff)
helps a lot if you don't want to stop and mess with settings .

I have several including one for cutting corrugated , You need a pretty fast Z but the DTHC will handle it if you set all of the tuning right.

[Deezl Smoke]

Oh,...in CommandCNC. Ok, I thought he was talking about 2 icons for sheetcam. Sorry. Old brain.
Ok, now that is some new info to digest. I had no clue something that could be done. So I can set up one for stainless then too. Give me a bit of time to re-read those instructions like several times.