Cut rules

More
27 Jul 2020 18:26 #176114 by CBEAR
Cut rules was created by CBEAR
Has anyone successfully written cut rules in sheetcam for plasmac? When I write cut rules for turning the thc on or off, the machine noticeably slows down at the cut rule and speeds back up after. I messed with the length before and after the rule to make sure that I wasn't just seeing a loss in velocity due to it being at a direction change. I removed velocity slow down cut rules to rule those out, and it's at every cut rule it slows the table down. Any ideas why it would do that? I would like to be able to turn the velocity down to 80% on corners along with the thc on and off. The thc on and off works great, but it's slowing down when it gets to those points.

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

More
27 Jul 2020 20:06 #176143 by rodw
Replied by rodw on topic Cut rules
I have used the hole cutting rules by attaching a rule set to the sheetcam plasma operation. I have posted it somewhere on the forum with some screen dumps but I could not find the thread. Plasmac has its own automatic version of hole processing and you can change the velocity slowdown applied.

Can you advise how you are applying the slow down and what gcode you are using?

Plasmac is not Mach so I don't think its necessary to embed specific cut rules into the job itself.

I have a slow project that should take this out of gcode altogether. I have modified the Linuxcnc core code to add real time pins that report the arc radius and if the arc is a hole or not in hal. This will enable much more sophisticated hole and arc processing so a separate component could apply a dynamic adaptive feed rate override based on some algorithm (which could be as simple as using the lincurve component).

Some high end controllers do centripetal limiting based on the arc radius that can be traversed at the current cut speed without slowing down. I think I finally have the maths right to do this and need to confirm if the trajectory planner uses the same approach to calculate the velocity to slow to on tight arcs. I've asked a couple of others to review my maths before proceeding too far becasue on one (yet to be confirmed) observation, the Trajectory planner is a long way off my calculated values.

So if there are any mathematicians here, please hold up your hand as it would be great to get feedback on my maths..
The following user(s) said Thank You: thefabricator03

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

More
27 Jul 2020 22:31 #176154 by snowgoer540
Replied by snowgoer540 on topic Cut rules
I think what he's saying, is the simple act of turning the THC off will reduce the feed rate for a small portion, and the same thing happens when you turn the THC on again.

You could be cutting a 6" line, turn the THC off half way, it will slow up and then speed up again. Turn the THC on again, it will slow up temporarily then speed up again.

When I talked to him earlier he was going to make a video demonstrating the above.

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

More
27 Jul 2020 22:43 #176157 by rodw
Replied by rodw on topic Cut rules
I don't think I said anything but I think if you have a linear move and you break it into 2 with a M62, it probably pauses to execute it. This is what I set up but I don't often use it.




Attachments:

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

More
27 Jul 2020 22:43 #176158 by rodw
Replied by rodw on topic Cut rules
Attachments:

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

More
27 Jul 2020 22:45 #176159 by rodw
Replied by rodw on topic Cut rules
Attachments:

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

More
27 Jul 2020 22:47 #176160 by rodw
Replied by rodw on topic Cut rules
I don't think the hold THC commands are necessary as the corner lock will disable the THC for us anyway.

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

More
27 Jul 2020 23:12 - 27 Jul 2020 23:16 #176162 by phillc54
Replied by phillc54 on topic Cut rules
Are you using M62 and M63?

I see in the docs that M64 and M65 will break blending.

As Rod said, if your velocity is 80% then if it is below the VAD percentage (default 90%) in the config panel it will lock out THC.
Last edit: 27 Jul 2020 23:16 by phillc54.

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

More
27 Jul 2020 23:27 - 27 Jul 2020 23:28 #176165 by snowgoer540
Replied by snowgoer540 on topic Cut rules

Are you using M62 and M63?

I see in the docs that M64 and M65 will break blending.

As Rod said, if your velocity is 80% then if it is below the VAD percentage (default 90%) in the config panel it will lock out THC.


I'm still a bit fuzzy on the difference between synchronized with motion, and immediately.

EDIT: Also, one question about the VAD percentage, so it considers 100% feed rate the feed rate with no M67 applied? As opposed to 100% being when it reaches the commanded 60% of the material's feed rate... if that makes sense?
Last edit: 27 Jul 2020 23:28 by snowgoer540.

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

More
27 Jul 2020 23:41 - 27 Jul 2020 23:41 #176168 by phillc54
Replied by phillc54 on topic Cut rules

[I'm still a bit fuzzy on the difference between synchronized with motion, and immediately.

From my understanding:
Synchronised means motion continues on it merry way and when the next G1/2/3 move after the M62/62 is reached it will enact that code.
Immediate means motion moves along then stops, the M64/65 is enacted then motion start again


EDIT: Also, one question about the VAD percentage, so it considers 100% feed rate the feed rate with no M67 applied? As opposed to 100% being when it reaches the commanded 60% of the material's feed rate... if that makes sense?

This is the percentage of the cut feed rate of the current material.
Last edit: 27 Jul 2020 23:41 by phillc54.
The following user(s) said Thank You: snowgoer540

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

Moderators: phillc54
Time to create page: 0.150 seconds
Powered by Kunena Forum