G4 pause after a G1 move

More
13 Apr 2016 09:27 #73215 by bill516
I've used dxf2gcode to generate the gcode for a sheet of different parts I am cutting which involve a lot of right angles, is there any way to automatically insert a G4 command after a G1 command in the code, or is there another way to do it i.e. in computing parlance if G1 then add G4

Bill.

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

More
13 Apr 2016 12:01 #73223 by andypugh
Replied by andypugh on topic G4 pause after a G1 move
You could probably use an input filter to do it.

linuxcnc.org/docs/2.7/html/config/ini-co...html#_filter_section

However I do not understand why you think you need this. Can you explain?

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

More
13 Apr 2016 12:57 #73226 by bill516
Replied by bill516 on topic G4 pause after a G1 move
At present the g-code that dxf2gcode generates cuts the corners giving a rounded corner instead of a corner that is just the cutter radius on inside corner or 90 deg on an outside corner. Inserting a G4 pause at the end of a line with G1 in it causes the cutter to pause and so makes the cut more of a 90 deg cut, than a radius which it does at present.

I've attached two files one with the G4 and one without, If you run them and watch the display you will see than the G4 cuts more of a 90 deg corner than the one without.

This is only a small file the actual file I have has maybe a couple of hundred 90 deg corners in it
Attachments:

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

More
13 Apr 2016 13:06 #73227 by andypugh
Replied by andypugh on topic G4 pause after a G1 move
It sounds to me as though your machine acceleration numbers could usefully be higher.

Then look at: linuxcnc.org/docs/2.7/html/user/user-con...c:trajectory-control

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

More
13 Apr 2016 13:41 #73229 by Todd Zuercher
Do you know how to use G64 and G61 correctly?
linuxcnc.org/docs/2.6/html/gcode/gcode.html#sec:G61-G61_1
linuxcnc.org/docs/2.6/html/gcode/gcode.html#sec:G64
Normally Linuxcnc defaults to plain G64 (maximum speed with blending) which will round corners terribly. Especially on a machine with low accelerations. Usually best results are achieved with G64 PXX where XX= a blending tolerance of how closely the machine must follow the programed path. G61 is exact path mode and replaces G64 and the machine will follow exactly the programed path (comming to a complete stop at each corner like you are asking for.)

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

More
13 Apr 2016 14:20 #73230 by bill516
Replied by bill516 on topic G4 pause after a G1 move
Thanks guys, G61 is the magic number that will do what I need for the time being.

There's more to this g-code stuff than meets the eye.

Bill

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

More
13 Apr 2016 14:27 #73232 by Todd Zuercher
May I suggest that you experiment a little with G64 as well. You may be surprised how much faster a file may run with say G64 P0.001 vs G61 on your machine without appreciably sacrificing part shape, and possibly improving surface finish and tool life through better speed management.

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

More
13 Apr 2016 21:24 #73256 by bill516
Replied by bill516 on topic G4 pause after a G1 move
Thanks Todd I will certainly give it a go. I keep learning new ways to do things, soon I might even know what I'm doing

Bill

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

Time to create page: 0.142 seconds
Powered by Kunena Forum