Another plasma component...

More
11 Jul 2019 09:36 #139086 by rodw
Replied by rodw on topic Another plasma component...
I just shared some info on external offsets for our plasma primer

Please Log in or Create an account to join the conversation.

More
11 Jul 2019 10:03 - 11 Jul 2019 10:03 #139092 by thefabricator03

I have had the torch airflow running after the cut but when I go to probe I get the ohmic probe detected while moving to probe height error.

Hmm, airflow "shouldn't" have any effect on probe detection, I don't know why that would be...


I think the cause was that there was already water inside the shield and it could not get out before the Ohmic probe detect feature came on. The air flow must not have been enough to remove all the water bridging the nozzle and shield.

When that was happening If I took off the shield and blew it dry it would work again.
Last edit: 11 Jul 2019 10:03 by thefabricator03.
The following user(s) said Thank You: phillc54

Please Log in or Create an account to join the conversation.

More
11 Jul 2019 10:14 #139095 by tommylight
The air fllow remains on 15 to 30 seconds after the torch is off, always in all plasma cutters.
The following user(s) said Thank You: phillc54, thefabricator03

Please Log in or Create an account to join the conversation.

More
11 Jul 2019 14:13 #139104 by islander261
Guys

The ohmic probe tripped while moving is the most common cause I have for stoppage. It is always caused by either water or slag (dross) shorting the nozzle to the shield. It is particularly bad when using the Finecut consumables because of the large gap between the shield and the nozzle. Many times I can fix the problem with just a finger over the shield opening while the post flow is still on using the airflow to blow the water out then restarting with the pause/resume button. If that doesn't work then I have to take off the shield and clean/dry between the shield and nozzle. A way to change probing methods from Gcode and the GUI will be a big help for the job shop crowd. I am stuck with ohmic because of the thinish material I cut.

'03

I figured that the standard consumables would be much less susceptible to this problem. I think when you put the anti dive snippet in your CAM before the end of cut it will help but not eliminate this problem. You can also increase your safe height so the torch travels higher on rapids. On the thicker material you are cutting at slow speed you really have no need for ohmic sensing anyway so just use the float switch. I am sure this is why HT has at least two probing methods on their machines Z axis. Sorry you had so much trouble getting the Z speed and accelerations correct. I think that many of us that have been around the EO branch just take the correct setup for granted.

John
The following user(s) said Thank You: phillc54, thefabricator03

Please Log in or Create an account to join the conversation.

More
14 Jul 2019 23:59 #139339 by docwelch
Phill,

I'm working on a post processor for Fusion 360 and just wanted to be certain I have this straight regarding the use of the M67 code. I'm working on a way to slow down cutting and stop THC compensation for small circles. For whatever reason, Fusion 360 CAM in the cutting 2-d profiling mode for plasma does not seem to always use a G2/G3 to do circles but rather makes a number of small linear moves. I was planning on just adjusting the speed by looking at the radius of the circle but that is not an option so I am having to think about alternate methods. Right now, I have something that might work though it is going to be a little unconventional in the g-code it creates. Please consider the following g-code snippet:

F#<_hal[plasmac.cut-feed-rate]>
M67 E3 Q60
F#<_hal[plasmac.cut-feed-rate]>

The first command would read/set the feed rate and the second would change it to 60%. My question is, what will that third command do? Will it reset back to the original feed rate or will it be essentially ignored? When I read the documentation, I'm led to believe that you have to do an M67 E3 Q100 to get back to the original feed rate.

Thanks for the help. I'll be happy to share my post processor if I can get it working.

Steven

Please Log in or Create an account to join the conversation.

More
15 Jul 2019 00:33 #139340 by rodw
Replied by rodw on topic Another plasma component...
Steven, at the end of the hole, do a M67 E3 Q0 to restore adaptive feed to 100% I don't think the feedrate will do what you expect with adaptive feed active. See linuxcnc.org/docs/devel/html/plasma/plas...user-guide.html#_thc

(So cool to have documents to refer people to :) )
The following user(s) said Thank You: docwelch

Please Log in or Create an account to join the conversation.

More
15 Jul 2019 00:37 #139341 by rodw
Replied by rodw on topic Another plasma component...
Here is a complete snippet for an example
  (Part: laser bracket)
  (Operation: Outside Offset, 0, T2: A120 Mild Steel 40 amp, 2mm [108V, 5.2 bar])
  M190 P2
  M66 P3 L3 Q1 
  F#<_hal[plasmac.cut-feed-rate]> 
  M3 S69
  G1 Y2.850
  M67 E3 Q70 (70% of cut speed)
  G2 I0.000 J1.650
  M67 E3 Q0 (100% of cut speed)
  M5

Please Log in or Create an account to join the conversation.

More
15 Jul 2019 01:45 #139344 by thefabricator03

Guys

The ohmic probe tripped while moving is the most common cause I have for stoppage. It is always caused by either water or slag (dross) shorting the nozzle to the shield.


With my old CandCNC feather touch ohmic probe I did not have these problems given the exact same running conditions,

I am not that great with electronics but I have read something in the past that said the big manufactures have a way to set the sensitivity of the Ohmic probe circuit, How would something like that work for our setup?

Please Log in or Create an account to join the conversation.

More
15 Jul 2019 01:48 #139345 by phillc54

The first command would read/set the feed rate and the second would change it to 60%. My question is, what will that third command do? Will it reset back to the original feed rate or will it be essentially ignored? When I read the documentation, I'm led to believe that you have to do an M67 E3 Q100 to get back to the original feed rate.

Yes, you need an M67 E3 Q100 (or Q0) to get back to the full feed rate.
The M67 E3 Qn code acts as a feed override to the current F word, so whatever feed is specified by the F word will be multiplied by the percentage of Qn.
The following user(s) said Thank You: docwelch

Please Log in or Create an account to join the conversation.

More
15 Jul 2019 01:53 - 15 Jul 2019 01:53 #139346 by phillc54

Guys

The ohmic probe tripped while moving is the most common cause I have for stoppage. It is always caused by either water or slag (dross) shorting the nozzle to the shield.


With my old CandCNC feather touch ohmic probe I did not have these problems given the exact same running conditions,

I am not that great with electronics but I have read something in the past that said the big manufactures have a way to set the sensitivity of the Ohmic probe circuit, How would something like that work for our setup?

Is the feather touch a separate piece of hardware?
Last edit: 15 Jul 2019 01:53 by phillc54.

Please Log in or Create an account to join the conversation.

Moderators: snowgoer540
Time to create page: 0.186 seconds
Powered by Kunena Forum