Need help in Incremental Round Move

More
19 Nov 2015 16:29 #65516 by G0G53Z148
Dear Linuxcncusers.

I am using Linuxcnc since 5 years and never get a problem like this.

I Want to move an Radius incremental with an predfined angle. I set the I and J of the Radius with G90.1 to absolut. But this will not do what i want.

I have seen the documentation with polarcoodinates and think this must be helpfull buts not true.

The workpiece is evry pice not similar to the others and there are 100 of this. The angle of Radius and the angle of the side are not the same. On my machine at Work with Heidenhain control is no problem to do this on it.

A sample it looks like this code
L X-36 Y-62 R0 FMAX
L Z2 R0 FMAX
L X-24 Y-62 RL F800
L Y-10
CC X-14 Y-10
CP IPA -70 DR-
L X0
L Y-55
L X-40
The Movement on X Axsis i havent implementet.

And as Sample now my Code wich i have done on Linuxcnc
o1010 sub
G90.1 (Radius Center Absolut)
G0 X-50 Y-65
G0 Z2
G1 G90 Z#4010 F#3001
(DEBUG, Tiefe soll #4010)
G1 G90 G41 X#4005 Y-60
G1 y-10

G02 G91 ^-112 I-14 J-10( CW Move define Angle)

G1 G90 X0
G1 Y-55
G1 X-35 
G90
G0 Z2
#4005=[#4005+#4006]
G40
o1010 endsub

For Better Understandig i Post the Complete Code and Drawing and as sample some Pieces of the Projekt.

Does anyone have a Idea ho to do this easy without CAM and without draw each point in CAD to messure the endponts of Radius.

Sorry for my English buts not my Native.

thank you and have a nice day
Roland

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

More
20 Nov 2015 00:17 #65551 by andypugh
polar coordinates use the current (X,Y) zero as the centre point.

So, you either have to set a temporary zero position at your chosen centre, or use some trigonometry.
LinuxCNC G-code has Sin, Cos and Tan functions.

Polar coordinates does help, try this code:


G90.1 (Radius Center Absolute)
G0 X200 Y200
G92 X0 Y0 ; This is our new centre point
G0 X50
G90.1 ; absolute circle centres
G2 F2000 ^-112 I0 J0 ; 112 degree move around the new 0,0 point
G92.1 ;cancel the temporary offset
m2

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

More
22 Nov 2015 06:31 #65645 by G0G53Z148
Thank you andi

i have found a other reason.
In you code i think i have tio left contour parth and move back

its bad that Linuxcnc can this not with simple commands

on my Heidenhein the code has 26 lines in Linuxcnc 120 ok there are 40000 dollars diffrent. :dry:

mai be some developer read this. Pleas add simple arc round for in and outside like Mach3 or others this will be verry verry helpfull.

thanks for reading

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

More
22 Nov 2015 21:56 #65673 by andypugh

Pleas add simple arc round for in and outside like Mach3 or others this will be verry verry helpfull.


What does the Mach3 G-code look like?

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

More
23 Nov 2015 06:45 #65687 by G0G53Z148
I dont use mach 3

I see it by e collegue. He wrote the ege of the pice with x20 r2
Y-10 r2
X0 r2

So the edge are round without i and j and correct endpoint

This function is verry helpfull at miling. At work i use them 100 times a day

Greetz

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

More
23 Nov 2015 12:23 #65695 by andypugh

Y-10 r2
X0 r2

So the edge are round without i and j and correct endpoint


You can use R to define an arc in LinuxCNC. That very same G-code will work in LinuxCNC.

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

More
23 Nov 2015 14:38 #65699 by G0G53Z148
i think we discuss different things

Linuxcnc must use g2 for round

At work HH uses after linear move R and the arc will be roundet
linuxcnc must tolt G2 <where to travel> < Radius>

User must Calculate the start and endpoint
if move will be longer or shorter Radius must be recalulatet

when CAM is used there is the radius in clear

i like oldschool and have not cam to use

i think this explain what i mean
try it
download the trial and use then you understand what i mean

HAND

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

More
23 Nov 2015 15:28 #65701 by andypugh
[quote="G0G53Z148" post=65699Linuxcnc must use g2 for round[/quote]
Or G3

At work HH uses after linear move R and the arc will be roundet
linuxcnc must tolt G2 <where to travel> < Radius>D


If you only specify a radius, does the system always assume the short arc?

With only a start and end point and radius there are always two solutions, or none.

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

More
23 Nov 2015 16:44 #65704 by jepler
It sounds like you're describing a fillet operation. You're right that LinuxCNC's gcode dialect does not support this.
The following user(s) said Thank You: G0G53Z148

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

More
23 Nov 2015 18:57 #65711 by G0G53Z148
jepler ! you are right ;)

english i snot ma native but you have checkt it thank you

@ andy i dont want spezifie an g2 or g3 move now it was the discuss abou arc rounding


example
linuxcnc
G91.1
G1 G41 Y0
G1 X9
G2 X10 Y-1 I0 J-1
G1 Y-9
G2 X9 Y-10 I-1 J0
G1 X-5
G40

other cnc Terivat
G1 G41 Y0
G1 X10 R1
G1 Y-10 R1
G1 X-5
i hop this is now clear for you what does i mean

Linuxcnc is a Goog controller but some thisgs are very very cumbersome :woohoo:

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

Time to create page: 0.090 seconds
Powered by Kunena Forum