Hello World - test cuts using new LDR Motion Systems table

[Diesel]

My LDR Motion Systems table is filled, leveled and up and running.
I've cut a few things so far with varying results...mostly good despite my inexperience with CNC plasma.

After doing some reading here on the forum, I need to adjust:
Air pressure - my pressure switch is non-standard (80-120 PSI ) - PM85 needs 90 PSI as a minimum, 135 PSI max. I need to fix this ASAP.
Setup and use my Ingersoll Rand D18IN (11 SCFM rated) refrigerated air dryer
Lead-ins/lead-outs - arcs may not be best for my machine
DTHC-IV tuning - after video review, I can see the Z axis diving in the middle of the cut...perhaps when it encounters dross from a previous pierce?

Despite my cut quality issues, I'm very pleased with the table. I honestly don't think you'll find a better built table for the money.

LDR was able to build me exactly what I wanted. I wanted the ability to cut and scribe on the rotary. They went one step further and made this possible without detaching the torch and using an extension arm. LDR made a custom aluminum gantry (to keep weight down), used linear bearings and I also have a full 5-axis CandCNC controller. No need to disconnect/reconnect anything at all...just park the gantry for either table or rotary use and I'm off to the races.

Here's a video showing a T3 turbo flange being cut in 1/2" steel.
Obviously I need to make some changes to my setup as well as the toolpath(s), but I'm learning!
https://youtu.be/s7KkXMvzBlM

Many thanks to those on this site for their file sharing and helpful advice. I'm really looking forward to getting 'er dialed in and making quality parts!

Cheers,

Matt

[Diesel]

Update:
After turning the DHTC off, my bevel has decreased significantly and the edge quality also improved.
...more tuning!

Cheers,

Matt

[acourtjester]

you may need to run test straight line cuts to find out if the DTHC voltage may need to be adjusted to get the correct cutting height.
Do cuts about 6" long and stop (hit reset button) after about 3" of travel and check the torch height. Change the set voltage and cut again and check to see if it is better repeat until the correct cut height is attained.

[Diesel]

Good call!

I did the voltage test and found that the preset/Hypertherm value of 127V for 1/4" steel at 65A was causing my torch to be too high during the cut - I didn't measure it, but estimate it was about 0.080" - 0.090".

I adjusted the voltage down to 125V and had the proper 0.060" cutting height.

I also ran my test part (simple T3 turbo flange) and while it did cut the bolt holes better than before, the bevel is still present on two sides of the cut.
Based on this, I'm thinking I have worn consumables. They looked OK to me when I checked them yesterday (bear in mind I've only done very rough manual plasma cutting previous to this), but based on the troubleshooting image I found, it's another variable to eliminate.

The fact that I can get nearly no bevel on one side (good enough to allow the part to stand on end) is encouraging.

I'm also investigating methods to eliminate the divots on the lead-in/lead-out for the larger contours.

Cheers,

Matt

[Brand X]

Are you cutting the outside of the piece Clockwise? Does not look like it in the pics. I have seen just about perfect examples from a Hypertherm 85 cutting .500 using 65 amp consumables.. 30 ipm book speeds..

[acourtjester]

Use the search function at the top of the page there are many posts covering divots and lead ins. You can read them instead of waiting for a reply. some work on the path rules may help too.

[dhelfter]

Matt,
Couple of things:
I would lower your water level a bit. We have not seen any advantage to running water that high on thicker plate. Lowering water will help with dross.

Are you cutting the holes at 50-60% of book speed with thc off?

When cutting, you can watch the z axis DRO and it will show the height (adjusts rapidly, but look at the average) you can then click lower volt or raise volt button on screen till it is consistently around.06" This voltage would then be your ideal voltage, and should be entered in sheetcam. Or you can do straight line tests like we discussed when you picked machine up. Either way, the key thing to remember is the height is what matters, not the voltage.

Your lead in and out's look like they need some work. I would play with some rules, such as slowing down at end of cut and maybe increase the leadout and add some overcut.

I also agree with brandX it appears you are cutting the wrong direction. Inside should be counter clockwise, and outside clockwise.

If after playing with these things, if you still are not getting good cuts, give me a call. We may need to adjust motor tuning in Mach3, as you have a one off gantry.

Thanks
Dan
LDR

[dhelfter]

One more thing. Make sure your z switch offset is correct. On thicker plate it does not take many pierces to close to ruin the consumables. I would also make sure torch is fully piercing material before any down movement. Here at our shop we actually increase the pierce delay by .1 to .2 of a second on thicker material.

Thanks
Dan
LDR

[Brand X]

You also might want to look at the speed of the Z when it sets the offset. Meaning if it's two fast, it might not be a consistence number each time.. I am sure every Z is a bit different in how it responds there..

[Diesel]

Whoa - lots of good responses. Thanks guys!

Are you cutting the outside of the piece Clockwise? Does not look like it in the pics. I have seen just about perfect examples from a Hypertherm 85 cutting .500 using 65 amp consumables.. 30 ipm book speeds..

Yeah, about that... It's entirely possible.
I noticed the 'reverse direction' option in SheetCAM and fear that it might have been enabled when it shouldn't have been.
By default, I thought SheetCAM took care of the cut direction automatically since you're telling it outside/inside contours. It would appear that I was mistaken about that. Before a test cut yesterday afternoon, I noticed the toolpath didn't look right - sure enough, it was going in the wrong direction. I am now double/triple checking my options before cutting. Sigh.

Use the search function at the top of the page there are many posts covering divots and lead ins. You can read them instead of waiting for a reply. some work on the path rules may help too.

That's on the to-do list!
That's exactly how I found some helpful info on the bevel issue. This forum has been great!

Matt,
Couple of things:
I would lower your water level a bit. We have not seen any advantage to running water that high on thicker plate. Lowering water will help with dross.

Are you cutting the holes at 50-60% of book speed with thc off?

Dan! Thanks for getting back to me!
Will do - I've been experimenting with the level. I've read that so long as it isn't 1" below the top of the slats, I'll be good to go in terms of keeping the smoke down.

Yes. For the small bolt holes, I reduced speed by 60% and turned off the DTHC.
I also increased my lead in so that it was at least in the middle of each hole.

When cutting, you can watch the z axis DRO and it will show the height (adjusts rapidly, but look at the average) you can then click lower volt or raise volt button on screen till it is consistently around.06" This voltage would then be your ideal voltage, and should be entered in sheetcam. Or you can do straight line tests like we discussed when you picked machine up. Either way, the key thing to remember is the height is what matters, not the voltage.

Your lead in and out's look like they need some work. I would play with some rules, such as slowing down at end of cut and maybe increase the leadout and add some overcut.

I also agree with brandX it appears you are cutting the wrong direction. Inside should be counter clockwise, and outside clockwise.

If after playing with these things, if you still are not getting good cuts, give me a call. We may need to adjust motor tuning in Mach3, as you have a one off gantry.

The Z axis varies quite a bit - it takes it quite a while to settle in at .060" when I've watched it...and sometimes it never does. I haven't tried to cut large parts with longer cuts yet since I'm trying to get it tuned before starting real production work.

In the YouTube video I posted above, you can see the torch diving at one point when I don't think it should have. Perhaps this occurring once or twice has ruined my consumables. I have some 85A and finecut consumables on order...they should arrive this week from Harris/Baker.

No doubt - my lead ins/outs need a lot of work...haha
I've added upwards of .200 overcut, tried slowing down before the end and even decreased the torch-on delay at the end...that last bit helped with the divot, but it made it a son of a gun to remove the part from the rest of the plate.

One more thing. Make sure your z switch offset is correct. On thicker plate it does not take many pierces to close to ruin the consumables. I would also make sure torch is fully piercing material before any down movement. Here at our shop we actually increase the pierce delay by .1 to .2 of a second on thicker material.

I religiously check the Z offset every time I fire up (or restart) the CandCNC controller.
Good call on increasing the pierce delay - I will definitely try that.

You also might want to look at the speed of the Z when it sets the offset. Meaning if it's two fast, it might not be a consistence number each time.. I am sure every Z is a bit different in how it responds there..

DRO always reads .250" and when I check the Z offset clearance, it is consistently good.
Are you talking about when it indexes to the pierce height?

Here are some pics of the straight line test cuts with the DTHC enabled - very exciting stuff...I hope you're sitting down.

.500" plate

FullSizeRender (1).jpg (112.62 KiB) Viewed 3547 times

.500" plate

FullSizeRender (1).jpg (112.62 KiB) Viewed 3547 times

.250" plate

FullSizeRender (2).jpg (102.27 KiB) Viewed 3547 times

.250" plate

FullSizeRender (2).jpg (102.27 KiB) Viewed 3547 times

Here are some pics of a part I intend on producing - that same T3 turbo flange. This was a test cut I did over the weekend. Best cut in .500" plate I've had to date - too bad its incomplete. I had DTHC completely turned off and absolutely no rules applied at all. I'm thinking that the top dross left behind from the small bolt hole pierces is wreaking havoc with the DTHC when the torch gets close to the holes/dross. The 4 corners on the outside contour are clean as can be on this piece, but on other pieces where I've cut the bolt holes, it is jagged. The bevel on this piece is also some of the best I've seen to date as well.

FullSizeRender (3).jpg (129.49 KiB) Viewed 3547 times

FullSizeRender (3).jpg (129.49 KiB) Viewed 3547 times

IMG_8899.JPG (72.24 KiB) Viewed 3547 times

IMG_8899.JPG (72.24 KiB) Viewed 3547 times

IMG_8902.JPG (71.49 KiB) Viewed 3547 times

IMG_8902.JPG (71.49 KiB) Viewed 3547 times

IMG_8903.JPG (74.12 KiB) Viewed 3547 times

IMG_8903.JPG (74.12 KiB) Viewed 3547 times

Are there any standardized test shapes I should be cutting so that I can compare/contrast with others?

Thanks for getting back to me, guys!
We'll get 'er ironed out!

Cheers,

Matt

[Diesel]

FYI/FWIW:
I just measured the bevel on that good flange cut in .500" plate.
On a good side with very little bevel (visual inspection) it tapers about .005" from top to bottom (inside contour to outside contour).

I also measured the overall width (OD) on the straight areas of the long side at either end.
The outside contour longer straight areas are parallel to within .003".

Scary that I have to turn off the DHTC to make this happen...

Cheers,

Matt

[acourtjester]

Diesel
I think the Z switch offset dhelfter is talking about is in SheetCam in the post processor.

[Diesel]

We never had to adjust that offset in the post processor options. The only Z switch offset I've had to change was the one in Mach 3.

Attached are my current settings.
Sorry for the goofy cropped photos...I'm doing this from my phone.

I'm currently re-leveling my torch with a Bosch self-leveling dual plane laser...

Cheers,

Matt

[acourtjester]

I think G-code overrides mach setting in that case you may want to contact LDR on that to be sure.

[dhelfter]

The switch offset for our machine is set on the mach3 screen. We have found that if the switch ever gets damaged and needs to be replaced, sometimes the new switch will be slightly different. If switch offset is in the gcode, you would need to re generate all new code. By using a dro on the mach3 screen, we can easily change it and continue to use previously generated code.

Matt,
The fact you can get good cuts without thc and they are not so good with thc says several things to me.
1. motion is acceptable
2. torch is perpendicular to plate
3. dthc needs tuning!!

On the mach3 screen is a button labeled dthc settings. If you click this, then the second tab you can adjust sensitivity and tracking. Believe it or not, you may need to detune the dthc for thicker plate.

Thanks
Dan
LDR

[dhelfter]

Matt,
Just watched the video again, it appears to "dive" after the pierce then lift up. This indicates to me that you need to increase the dthc delay in sheetcam tool. I think it is pierceing and dthc is "kicking" in before it has moved completely away from the pierce area. This will make voltage read high, and force z axis down, hence the split second dive.

In sheetcam, leave reverse cut direction selected (has a check mark) and machine will go the correct way.

as for taper, .005" on 1/2" material is 1 degree. Not sure you will consistently get any better with air plasma
Also I don't believe there is a need for a super precise level/square needed to set up torch. Unless you are going to do it very time you cut, it is going to change slightly as the deck gets "chewed up".
Thanks
Dan
LDR

[Diesel]

The switch offset for our machine is set on the mach3 screen. We have found that if the switch ever gets damaged and needs to be replaced, sometimes the new switch will be slightly different. If switch offset is in the gcode, you would need to re generate all new code. By using a dro on the mach3 screen, we can easily change it and continue to use previously generated code.

This makes perfect sense. I actually found that the v-rollers on my Z axis needed to be adjusted after the long journey home. Yesterday, I adjusted them and originally had them too tight and saw that the torch plate was not resting all the way down on a consistent basis - so that messed up my torch height and DTHC as well.

Matt,
The fact you can get good cuts without thc and they are not so good with thc says several things to me.
1. motion is acceptable
2. torch is perpendicular to plate
3. dthc needs tuning!!

On the mach3 screen is a button labeled dthc settings. If you click this, then the second tab you can adjust sensitivity and tracking. Believe it or not, you may need to detune the dthc for thicker plate.

I agree - the motion appears to be good.
The torch was off a bit - gantry had to be removed for transport. But now I've corrected that.
I have not done a test cut after properly adjusting the torch and torch plate v-rollers. I worked my "day job" from 2PM yesterday until 7AM today.
I will have a look at these settings ASAP - I'm back on the road again tonight for work...good times.

Just watched the video again, it appears to "dive" after the pierce then lift up. This indicates to me that you need to increase the dthc delay in sheetcam tool. I think it is pierceing and dthc is "kicking" in before it has moved completely away from the pierce area. This will make voltage read high, and force z axis down, hence the split second dive.

OK, I will tweak that. I believe it is set to 1.3 seconds.

In sheetcam, leave reverse cut direction selected (has a check mark) and machine will go the correct way.

So I can leave that checkbox selected all the time?
In SheetCAM, I've been paying closer attention to the cut path direction and I've had to go back and check/uncheck this to ensure the path as shown is CCW for inside contours and CW for outside contours.

as for taper, .005" on 1/2" material is 1 degree. Not sure you will consistently get any better with air plasma
Also I don't believe there is a need for a super precise level/square needed to set up torch. Unless you are going to do it very time you cut, it is going to change slightly as the deck gets "chewed up".

Heck yes - I can definitely live with that taper if it was consistent on inside/outside contours. It's when the taper is bad enough that the part can't stand on end without falling over that I have a problem. I have a customer that currently sends a lot of work to a laser shop - I'll never compete with a laser, but I can sure as heck try to get it close.

I bought that Bosch laser at Home Depot for home remodeling projects - it has been very handy. We shall see soon if it has helped with my torch alignment.

Lasty, am I expecting too much on those small bolt holes in .500" plate?
I read somewhere (probably here on the forums) that its hard to do precise holes when the hole is smaller in diameter than the thickness of the material.

Thanks, as always, Dan!

Cheers,

Matt

[Diesel]

Pic of the consumables...for what it's worth...

Cheers,

Matt

[Brand X]

So I can leave that checkbox selected all the time?



Yes..

[dhelfter]

Matt,
On page 5-3 of your hypertherm manual, it gives information on inspecting consumables. Hard to tell in the pic because of the angle, but the nozzle looks like the hole is round, that is good. The electrode does look to be eaten down some, again hard to tell in a picture, but they don't look that bad.


As for holes, I don't know if I would say you are expecting to much, but in our experience a hole smaller in diameter than thickness of material is hard to remove all the taper.
Dan
LDr

[Diesel]

So I can leave that checkbox selected all the time?

Yes..

Done! Thanks!

Matt,
On page 5-3 of your hypertherm manual, it gives information on inspecting consumables. Hard to tell in the pic because of the angle, but the nozzle looks like the hole is round, that is good. The electrode does look to be eaten down some, again hard to tell in a picture, but they don't look that bad.
As for holes, I don't know if I would say you are expecting to much, but in our experience a hole smaller in diameter than thickness of material is hard to remove all the taper.

Thanks, Dan. I went ahead and replaced the nozzle and electrode anyway.
I agree that they didn't look all that bad given my experimentation. Especially compared to other plasma cutters I've used in the past.

That's what I thought I had read before. Thanks for clarifying that!

I've temporarily switched my focus from tuning the DTHC to removing the divots at lead-in.
The cuts are just awesome everywhere but the lead-in. Time for some research!

Thanks again, guys!

Cheers,

Matt

[Diesel]

Here's a part I recently drew up to test some parameters.
2" OD with 1" ID in 1/2" steel.

I can't seem to get rid of the damn divots. ID is set to cut at 60% speed.

I've recently changed my acceleration up a bit - no change...so I may try slowing it down from the OEM setting.
I've also experimented with pierce delay, delay at end of cut, etc.
Everything except for the pierce/lead-in area is cutting beautifully!

Washers.jpg (34.24 KiB) Viewed 3381 times

Washers.jpg (34.24 KiB) Viewed 3381 times

Washer_ID.jpg (21.76 KiB) Viewed 3381 times

Washer_ID.jpg (21.76 KiB) Viewed 3381 times

Cheers,

Matt

[dhelfter]

Matt,
what type of leadin and out were these cut with? I would try perpendicular lead in and lead out with .060 over cut

Dan
Ldr

[comeoutswingin]

Here's a part I recently drew up to test some parameters.
2" OD with 1" ID in 1/2" steel.

I can't seem to get rid of the damn divots. ID is set to cut at 60% speed.

I've recently changed my acceleration up a bit - no change...so I may try slowing it down from the OEM setting.
I've also experimented with pierce delay, delay at end of cut, etc.
Everything except for the pierce/lead-in area is cutting beautifully!

Cheers,

Matt

I've been watching this, because I'm pretty stoked to be getting my LDR table here pretty soon. I have a Torchmate 4x4 now and I wanted to show you this. These are cut from 1/4" HR with a 90 Lead in of about .75". 65 Amps with a powermax 85. What you're getting imo is pretty good, esp for 1/2" material. I think you're getting the divots because of the 90 degree lead in. The machine has to make a 90 direction change. For a basically immeasurable moment, one axis stops and the other starts. In that super small window I think the arc goes from a trailing arc to a vertical, maybe even a leading arc. Try using an angle on your lead in, maybe even an arc. The over cut feature would be something I would try on holes or circles. You can see in my picture that I have divots, but in the corner where the direction changes at much less of an angle, it seems pretty good.

I don't know if adjusting your acceleration rates will really do much for you. I believe its mostly arc wander or deflection.

[Diesel]

Matt,
what type of leadin and out were these cut with? I would try perpendicular lead in and lead out with .060 over cut

I've tried:
Upwards of .4" arc lead in
Upwards of .3" perpendicular lead in
Upwards of .200 over cut
I have tried most of the same with lead outs...but did not get as wild with the length.

I've been watching this, because I'm pretty stoked to be getting my LDR table here pretty soon.

I know the feeling! You won't find a better built table out there. I looked a LOT and and am certainly happy with my purchase from Dan and his brother.

These are cut from 1/4" HR with a 90 Lead in of about .75". 65 Amps with a powermax 85.

.75" lead in? That's a big lead in!
.4" has been my limit so far.

What you're getting imo is pretty good, esp for 1/2" material. I think you're getting the divots because of the 90 degree lead in. The machine has to make a 90 direction change. For a basically immeasurable moment, one axis stops and the other starts. In that super small window I think the arc goes from a trailing arc to a vertical, maybe even a leading arc. Try using an angle on your lead in, maybe even an arc. The over cut feature would be something I would try on holes or circles. You can see in my picture that I have divots, but in the corner where the direction changes at much less of an angle, it seems pretty good.

I don't know if adjusting your acceleration rates will really do much for you. I believe its mostly arc wander or deflection.

I agree. It's expecting a lot from the machine.

My cuts in 1/2" (note with DTHC disabled) definitely are pretty good.
Am I being picky?
Yup.
However, I've seen what air plasma is capable of when its tuned right and see no reason to expect any less.

I cut some 1/4" @ 85A this afternoon (yes, I know...WAY too much power) and the divots were worse...as you'd expect with the torch moving around at 130 ipm.

I did some research this morning and found where a few folks (including Jim Colt) suggested that perhaps the gantry acceleration should be changed to help avoid the divots. My divots definitely got worse when I bumped up the acceleration, but they did not get noticably better when I bumped it down the same amount in the negative direction (passing the original which was 35 inches/sec/sec or ~.09 G's).

My gantry is a one-off custom - I expected the need to tune it a bit.

I have some 45A fine cut consumables to try out on some 16GA. I'm interested to see the results.

Cheers,

Matt