Sheetcam rule not being put in G-code on some operations. Ideas?

[motoguy]

I thought I had my "diving into the plate on small holes" issue figured out, but maybe it's not. I've set the Ref Distance to 0 in Sheetcam, forcing the ohmic to sense the plate at each pierce. I thought that fixed the issue I had before (ok, it DID fix it on the previous cut), but it appears to be back.

I've got a series of 8 holes to cut in 14ga hot rolled. First one cuts fine. Touches off plate, raises to .15, fires, pierce delay of .4 (was .2), drops to .06, cuts a great hole. THEN, when it moves to holes 2-8, when it drops to .06 for the cut, it proceeds to drive the torch into the plate. Initially all holes were on the same layer, and I thought maybe it was an issue with the "holes" rule (DTHC off, 65% feedrate, then DTHC back on). I then put the holes each in individual operations, and the problem persists. On the individual operations, I just did a copy/paste on the operations, so they're identical (aside from selecting different holes). Same "holes" rule selected, same content.

HOWEVER, if you look at the Gcode, you see the S10 (DTHC off) command is on line 390 for the first hole, and S20 (DTHC on) on line 440. Looks good. The equivalent place on hole 2 would be lines 630 and 690, but it's not there.

Here is the code snipped for hole 1 (cuts fine), and hole 2. Touch off for first hole starts on line 290, touch off for second hole starts on line 530. Any ideas? It's been a long night, and so far it's been one of those days where everything that can go wrong, is...so maybe I'm missing something simple.

N0290 G31 Z -11.81 F20.0 (Start Probe Touch-Off )
N0300 G92 Z0.0
N0310 G00 Z0.002 (Switch Offset Lift)
N0320 G92 Z0.0
N0330 G00 Z0.150
N0340 M03
N0350 G04 P0.2
N0360 G01 Z0.060 F150.0
N0370 F90.0
N0380 X5.215 F270.0
N0390 S10 (THC OFF) (On small circles)
N0400 G03 X5.249 Y5.461 I0.035 J0.000 F148.5
N0410 X5.284 Y5.495 I-0.000 J0.035
N0420 X5.250 Y5.529 I-0.035 J-0.000
N0430 X5.215 Y5.495 I-0.000 J-0.035
N0440 S20 (THC ON) (On small circles)
N0450 X5.249 Y5.461 I0.035 J0.000 F270.0
N0460 X5.282 Y5.487 I-0.000 J0.035
N0470 (Operation: Inside Offset, mount hole 2, T5: 45 amp 14 gauge steel)
N0480 M05
N0490 G00 Z0.800
N0500 X5.254 Y6.739
N0510 M900 (Check for Z active)
N0520 G00 Z0.28
N0530 G31 Z -11.81 F20.0 (Start Probe Touch-Off )
N0540 G92 Z0.0
N0550 G00 Z0.002 (Switch Offset Lift)
N0560 G92 Z0.0
N0570 G00 Z0.150
N0580 M03
N0590 G04 P0.2
N0600 G01 Z0.060 F150.0
N0610 F90.0
N0620 X5.215 F270.0
N0630 G03 X5.249 Y6.705 I0.034 J-0.001
N0640 X5.284 Y6.739 I0.001 J0.034
N0650 X5.250 Y6.773 I-0.035 J-0.000
N0660 X5.215 Y6.739 I-0.001 J-0.035
N0670 X5.249 Y6.705 I0.034 J-0.001
N0680 X5.282 Y6.730 I0.001 J0.034
N0690 (Operation: Inside Offset, mount hole 3, T5: 45 amp 14 gauge steel)
N0700 M05

[Simko]

There is no code to turn the THC off for hole #2, maybe there IS something wrong with your 'Holes' rule or maybe the post. Just for the hell of it, try running with no THC.

[motoguy]

The THC did not turn off for hole #2.

Just saw that while reviewing the post/code. Any ideas why that would be? Can I manually go in and copy/paste into the appropriate place to get this part cut?

Verbage of "holes" rule: On circles smaller than 1.5in set feed to 65% and output Code: DTHC-OFF then output Code: DTHC-ON after the circle"

Post is DTHC-HYT-TAP_SoftPierce+Marker-rev11J" - CandCNC post.

ETA: The holes in question are .12" in size. First cuts fine...rest torch dives into plate. Previously smallest holes I cut were .177, and it did fine (after changing reference distance to 1, so ohmic touched off for each pierce). It cuts the first hole fine, so I know it can do it. Maybe it's something related to the hole size?

In my cut settings, "Min Cut Length for DTHC" is set at the default "1". DTHCIV response profile is at the default 1.

[motoguy]

I just noticed it's not slowing down the feed rate for the 2nd+ hole, either. Looks like the "holes" rule isn't being applied at all after the first hole...

[Simko]

This may sound like a crazy idea, but I just had a similar issue but with feed speed.

Generate the g-code again, but use a different tool (ie instead of 14 ga, try 12 ga or 16 ga) and see if the code generates differently and the Holes rule is applied to each hole along with feed speed changes.

[Simko]

I see you edited your first post to look like you knew that the THC was not turning on and in turn making me look like I didn't read your post...

[East German]

Hallo,

see in Sheet Cam Plunge safety clearence!

Is an idea!

[motoguy]

I see you edited your first post to look like you knew that the THC was not turning on and in turn making me look like I didn't read your post...

Ha! Not at all! I was editing it while you were posting your comment...when I saw that, I quoted your comment to make sure it was acknowledged.

[motoguy]

This may sound like a crazy idea, but I just had a similar issue but with feed speed.

Generate the g-code again, but use a different tool (ie instead of 14 ga, try 12 ga or 16 ga) and see if the code generates differently and the Holes rule is applied to each hole along with feed speed changes.

yeah. It appears to be an issue with implementation of the rule. I'll delete that rule, rebuild it, and see how it does. Based on your post above, I'll delete that tool and rebuild it as well. Thanks!

[acourtjester]

cold it be that your "rapid clearance" and the "Plunge safety Clearance" are to close I run my rapid clearance 1" (25.4 mm).
What is the rapid height when starting the cut operation?

[motoguy]

Rapid height was .8, plunge safety was .28. Those heights were in the machine when I purchased it. I changed rapid height to 2" -after- cutting this morning. Have not ran machine since the change.

[motoguy]

BTW, I manually disabled the THC while the table was cutting the small holes. It did fine. I was a bit disappointed with the hole roundness, until I realized it was not applying the % slowdown, either...so it was cutting these .12 holes (.055 kerf width), with a 45A shielded nozzle, at 45A on 14ga, at 270 ipm. Given that information, I was actually pretty impressed with the roundness. My last go-round with the Finecut nozzle wasn't that impressive (been running 45 since, as it cut better), but I plan on spending some time to measure cut height/voltages on the Finecut, and get it dialed in.

No idea why the rule information wasn't being applied to all the features of a layer in the same way, but I'll take a software setting vs a hardware issue any day of the week. Thanks for the assistance, guys.

[Simko]

Not saying that this is your issue, but I had a strange problem with the feed speed being set correctly for the first cut, but not being set correctly for all of the subsequent cuts. This only happened when I used Tool #1. Whenever I used any other tool, it would properly set the feed speed on all of the cuts. I raised the issue and Les from SheetCAM found it was an issue with the post processor.... So when you go to download the Rev 16 version of the CandCNC post, you can think of me.

[motoguy]

Not saying that this is your issue, but I had a strange problem with the feed speed being set correctly for the first cut, but not being set correctly for all of the subsequent cuts. This only happened when I used Tool #1. Whenever I used any other tool, it would properly set the feed speed on all of the cuts. I raised the issue and Les from SheetCAM found it was an issue with the post processor.... So when you go to download the Rev 16 version of the CandCNC post, you can think of me.

Did it happen when you use ANY setup as tool #1 (ie, changed the settings within the tool, and it still did it), or just with a certain config as tool one (ie, you changed a tool1 parameter, and the problem went away)? Wondering if changing a tool1 setting may fix the issue, or if tool1 in the list needs avoided completely (mine's a different tool, but let's use "tool1" as an example).

So when you go to download the Rev 16 version of the CandCNC post, you can think of me.

Rev 16...hmmm...where do you find such a beast? I just came back from the CandCNC page...lol

[tnbndr]

This only happened when I used Tool #1. Whenever I used any other tool, it would properly set the feed speed

May be worth a try. Leave your tool #1 as a decoy and recreate that tool further down the list and see if the rules apply to the new tool. If it works just rename Tool #1 as DO NOT USE.