Hello World - test cuts using new LDR Motion Systems table

[BensPlasmaAu]

Sorry to hijack your thread here Diesel, but does everyone run their z axis this quickly? Mine is a BUCKET load slower, by a factor of like 10. Am I wrong? Man this building your own table thing is confusing. It's good to have the LDR guys helping out.

[Diesel]

Sorry to hijack your thread here Diesel, but does everyone run their z axis this quickly? Mine is a BUCKET load slower, by a factor of like 10. Am I wrong? Man this building your own table thing is confusing. It's good to have the LDR guys helping out.

No worries at all - the primary reason I started this thread is so that myself and others can learn.

Sorry, I should have specified: the 35 inches/sec/sec is the X, Y, A acceleration.
My Z is set to 25 inches/sec/sec.

Your Z must be able to quickly index from pierce height to cutting height...say .018" to .060"...granted that distance is not like sending a man to the moon, but if you're 10x slower than that, I could see this causing you some issues such as bad cut path geometry (bevel) until its at the right cut height, reduced consumable life, etc.

Your DIY table may need different acceleration rates (and velocities) due to the weight of the gantry.
My gantry is a one-off custom since I wanted to cut and scribe on the rotary...but the weight is about the same (perhaps slightly less?) than a traditional steel gantry because it's mostly aluminum.

Cheers,

Matt

[dhelfter]

Matt,
Actually those acceleration numbers are in inches per second squared, not MM

Thanks
Dan
LDR

[Diesel]

Matt,
Actually those acceleration numbers are in inches per second squared, not MM

Oops!
Yeah, big difference!
I've updated my above post to avoid confusion.

Thanks!

Matt

[dhelfter]

Here are some pics of holes I just cut yesterday. Consumables had around 600-800 pierces on them. 85 amp in 1/4" mild steel.
.25" lead in .02" overcut and .07" arc lead out

[dhelfter]

Not sure what I am doing wrong? Pics are 300kb and won't upload?
Dan
LDR

[Diesel]

Very odd - here's a 1.2MB .PNG

[dhelfter]

trying again

[Diesel]

^ I'd be perfectly happy with that!^

I did a volt test this afternoon.
Had the voltage for .250" @ 85A all the way down to 115V (123 is ideal) to make the DTHC happy and end up close to an average .060" cut height.
The Z still creeps up from .060" towards the cut every freakin time. Starts out at .060...jumps around a bit...might average something close to .060" and then it its .11" to .18" or more at the end of the cut.

...then I tried a 'washer' test cut like you did and saw that my consumables were trashed...horrible bevel - bad nozzle.
DTHC strikes again!

So here's one I did a short while ago in .250" steel...new electrode and nozzle and with DTHC disabled.
I'm going to try one with your lead in / lead out - mine are set quite a bit bigger than what you have.

IMG_8989.JPG (89.53 KiB) Viewed 2616 times

IMG_8989.JPG (89.53 KiB) Viewed 2616 times

IMG_8990.JPG (85.2 KiB) Viewed 2616 times

IMG_8990.JPG (85.2 KiB) Viewed 2616 times

[dhelfter]

Matt,
Remember the dthc works a lot faster than what can be displayed on the screen. I think you are way over tweaking everything. This is what I suggest:
Just do straight line cuts (around 6-8 inches). Try and lay material on a flat area of slats. Generate code per book specs, except no thc, no lead in or lead out. Check the z switch offset before cutting. Make the cut, making sure plasma cutter has correct consumables installed and is set at correct amperage. While it is cutting watch the torch volts display. Yes it will vary widely at begining and end of cut, but should stabilize within 2 or 3 volts in the middle of cut. Now go back in to sheetcam and enter this voltage for that tool.
Re generate the gcode, this time with thc on. Re run the code, this time in the middle of the cut click stop. Now using a feeler gauge check that the torch is .060" from plate. I believe Hypertherm says you can have successful cuts with +/- .005" from .060" . I it is not within spec on distance, raise or lower voltage by one volt at a time and repeat. This works best with new consumables installed.

When you say the z creeps up, and the end of cut is .11 to .18 is this from the z axis dro on the screen, or actual measurement you are doing by stopping the program?

If possible, send me some gcode you are cutting, then cut it and video the mach3 screen. This would really allow me to help you more.

Thanks
Dan
LDR

[Diesel]

No doubt I've been tweaking.
I'll do your procedure in the AM provided I don't end up with a service call.

I'm always looking at the DRO. With the DTHC enabled, it very seldom is anywhere near the .060" cut height.
With the DTHC disabled, it's on lockdown right at the commanded cut height.

I'll get a video of the screen while cutting with the DTHC enabled and post it up on YouTube.

I'll send some G code now.

Here's some pics of the same part (DTHC disabled) with your parameters - overcut, lead-in and lead-out specified.
That blowout on the bottom is something I haven't experienced so far. Neat.

[Diesel]

This afternoon I cut out a unicorn for my wife's coworker from 16GA using 45A finecut consumables.
Honestly - I think it turned out pretty damn good considering it was only about 7" wide and 10" tall.
The inside contours weren't big enough for lead-ins...bummer.

Here's the post in another thread - so I could thank the gent for sharing the file.
http://www.plasmaspider.com/viewtopic.p ... 45#p103945

[Diesel]

Update:
I've done the volt test on .250" plate (@85A - the only other consumables I have are 45A Finecut...) - had to reduce the voltage a bit in order to have the DTHC track cutting height at 0.055-0.060".

Since I was more confident in the DTHC, I decided to cut some test "washers" again.
I also experimented with lead-ins, lead-outs as well as overcut to help eliminate the divots.

Of note, the geometry on the outside contour near the lead-out is distorted. It almost appears like the slag puddle from the lead-in is affecting the DTHC. (DTHC disabled on inside contour and feed rate reduced by 60%)

Here are some pics.
I've numbered each one with permanent marker and saved the g-code separately so that I can keep track of the results, share the code or reproduce it on my own table.

Cheers,

Matt

[comeoutswingin]

Update:
It almost appears like the slag puddle from the lead-in is affecting the DTHC.

Matt

This is why I have such a long lead in on my stuff.

[Diesel]

This is why I have such a long lead in on my stuff.

OK, that makes sense.
With this in mind, I think the slag puddles from the bolt holes were goofing up my other contours back when I was trying to cut those flanges with the DTHC enabled.

65A consumables are on order.
I really shouldn't be cutting 1/4" with 85A and expect perfection.

Thanks for your input!

Cheers,

Matt

[steel 35]

This is why I have such a long lead in on my stuff.

65A consumables are on order.
I really shouldn't be cutting 1/4" with 85A and expect perfection.

No 45s

[Diesel]

No 45s

I have 45A Finecut...but after looking in the Hypertherm book, that's only good to 10GA.
1/4" is well inside the 65A chart.

10GA through 1/4" is an area where I won't spend a lot of time...or so I think...

Cheers,

Matt

[dhelfter]

As Jim Colt has stated many times. The lowest amperage you can cut a given material at the best edge quality. Not saying you can't cut at the higher amperage, but expect better edge quality if you use lower amperage.

Dan
LDR

[steel 35]

No 45s

I have 45A Finecut...but after looking in the Hypertherm book, that's only good to 10GA.
1/4" is well inside the 65A chart.

10GA through 1/4" is an area where I won't spend a lot of time...or so I think...

Cheers,

Matt

Not Fine cut! Just 45A last line is 1/4" They have been my fav.
Only problem will be watching it go that slow

[Diesel]

Results are in...

Cutting 1/4" @ 65A with 65A consumables does not provide a marked improvement in the divots. In fact its hard to distinguish between the 65A and 85A "washers" that I cut. I did the volt test on 1/4" @ 65A, cut with/without DTHC, etc.

Suffice to say that I'm frustrated.

[Diesel]

I cut a full 4x8 sheet of 1/4" tonight @ 65A.
Only issue I had was the DTHC - I have no explanation why it would be on 95% of time time on other cuts and off on some pretty big cuts...
The torch dove into the plate on the last cut - shield touching the plate kinda dive. Ouch. Consumables (mostly the nozzle) are done.

Bevel on large outside contours was pretty damn good.
Bevel/geometry on 1" ID holes could be better (same issues as before, but I expected that).

Here's a slow-mo video showing a cut from earlier tonight.
It seems like the torch is staying on a fair amount of time after the motion has stopped, right?

http://youtu.be/GBR-0oNvNe0

Here's my first fully nested 4x8 sheet. I was pleased with the outcome.
Next time, I'll have to allow some additional space when I zero the torch in Mach3 since SheetCAM likes to shift everything to the very edge.

IMG_9071.JPG (137.9 KiB) Viewed 2475 times

IMG_9071.JPG (137.9 KiB) Viewed 2475 times

Cheers,

Matt

[tnbndr]

Next time, I'll have to allow some additional space when I zero the torch in Mach3 since SheetCAM likes to shift everything to the very edge.

Yes, sheetcam moves everything in the drawing to 0,0, you can fool this by adding a couple lines in your CAD program at 0,0 on a layer that doesn't cut. Or what I do is zero the torch in Mach 3 and then move(jog) it in the X and Y .125 to give some room from the edge of sheet.

[Diesel]

Yes, sheetcam moves everything in the drawing to 0,0, you can fool this by adding a couple lines in your CAD program at 0,0 on a layer that doesn't cut. Or what I do is zero the torch in Mach 3 and then move(jog) it in the X and Y .125 to give some room from the edge of sheet.

Good tip!

I've done the jog after zeroing (...to give me some time so that I could hit Run and then hurry over to the table and start a video)...but it just rapids back to where the original 0, 0 point was and starts going to town.

I emailed Dan and he had a look at the SheetCAM job file as well as the .DXF. My CAD drawing had some open entities - so that's why the DTHC was not operating as expected...it was being commanded off on one cut and never commanded to turn back on.

From Dan:
"Sheetcam looked at each entity, and with the path rule (DHTC) off before end, was shutting dthc off, but nothing turned it on till the next pierce
point."

Lessons learned!

Cheers,

Matt

[Diesel]

Ha!
Take a look at the SheetCAM screenshot above.
Why would there be a rapid along the same line that should be one, continuous outside contour?! Because it's an open entity and SheetCAM allowed me to join them with the "Offset open paths" option!

Damn!

[acourtjester]

Not sure if this is what you are talking about for edge postioning.
Hight light the corner part or edge part when nesting and change the X & Y values to the distance away from the edge you want.
You can zero the torch on the edge and the cuts will happen the distance you entered from the edge