Blending of motion

[Zig]

Hello Board,


I have been playing with EMC for some time now running kernel 2.6.24-16-rtai.

My current problem is blending of motion.

I include G61 code in my ngc files an i still get significant blending ( read rounding of corners ) of motion.

This does not happen always. Sometimes I get expected results and yet at other times the results are awful.

I suspect my understanding of G code is superficial so here isthe question:

What to include at the start of the file to ensure G61 or G61.1 always work correctly.


To help any kind soul in the know here is a portion of the .ini file which might be relevant to this issue:

Typically coordinated motion takes place at 80 mm/second

Please advise if additional information is needed

[EMCMOT]
EMCMOT = motmod
SHMEM_KEY = 111
COMM_TIMEOUT = 1.0
COMM_WAIT = 0.010
BASE_PERIOD = 20000
SERVO_PERIOD = 1000000
TRAJ_PERIOD = 10000000

[TRAJ]
AXES = 3
COORDINATES = X Y Z
LINEAR_UNITS = mm
ANGULAR_UNITS = degree
CYCLE_TIME = 0.010
DEFAULT_VELOCITY = 40
MAX_LINEAR_VELOCITY = 1200
DEFAULT_ACCELERATION = 1500
MAX_ACCELERATION = 2000

[AXIS_0]
TYPE = LINEAR
HOME = 0
MAX_VELOCITY = 180
MAX_ACCELERATION = 750
STEPGEN_MAXACCEL = 1000
SCALE = 200.0
FERROR = 1.25
MIN_FERROR = .025
MIN_LIMIT = -0.4
MAX_LIMIT = 617.500
HOME_OFFSET = 64.00
HOME_SEARCH_VEL = -15.0000
HOME_LATCH_VEL = -0.50000
HOME_SEQUENCE = 1

Similar Threads:

• help with blending
• BST LINEAR MOTION-Professional Manufacturer for Linear Motion Products In China
• surface blending
• Blending algorithm of EMC2
• Ok Now what? No motion at all

[acondit]

I assume that you are talking about rounding on xy transitions?
What is you max_acceleration for the Y axis [AXIS_1]?

Alan

[Zig]

Hello Alan,


All three axes have identical motion parameters.

I did go back to the .ini file and had another look at it. The file did not contain the RS274NGC_STARTUP_CODE

It does so now G90 G61 G21. This does not mean I know what i am doing; its a bit of a hit and more of a miss situation.
I have put the machine through its paces a few times since and so far so good.

Wish I knew why.

[samco]

this has a good explaination.
http://wiki.linuxcnc.org/cgi-bin/emc...jectoryControl

strait g64 is going to try to touch every segment while trying to go as fast as it can (up to the current feedrate)

If your acceleration is set low - it will round corners quite a bit. I think your best solution is to use G64 Px.xxxx. x.xxxx is how close you want emc to follow the actual path. This mode does a few things.. It will blend line segments together within the desired tolerance. It also will slow down only enough to also keep the path within tolerance.

sam

[acondit]

Maybe that was the problem. Maybe somehow it was defaulting to some other mode.

Good luck,
Alan

[Zig]

Observations so far...


Starting EMC2 and loading Gcode file which contains G61 behaves initialy.

toggling machine power F2 button and reruning the program results in erronious performance that is G61 is ignored


Going into MDI and invoking G61 command sometimes works after F2.

G64 P command with a small setting almost approaches G61 performance and may be a suitable option.


QUESTION:

Is there a way of making EMC2 wake up in G61 default mode?

Is there a way of retaining G61 after F2 has been invoked?

[Zig]

In retrospect previos post is incomplete.. I am using AXIS gui

MDI ( F5 ) panel shows active G codes. G61 is active according to the display yet the motion is very much blended after machine power toggle ( F2 ).


Oh one other thing.. I am using AMD based PC Ubuntu 8.04 and 2.6.24-16 rtai kernel.
Is the OS compatible with the CPU? ( intel vs amd? )
Hope this is a bit clearer.

[Jeff Epler]

I found the cause of the bug you described and fixed it for the next release of emc2 which I hope will occur sometime in July.

For more details, you can look at the bug tracker item I created about this problem:
https://sourceforge.net/tracker/inde...44&atid=106744

[Jeff Epler]

Until the next release, you can probably work around this bug by putting the following sequence at the top of your gcode programs:
G64
G61
Even after the next release this sequence will be OK and shouldn't cause any problems.

[Zig]

Jeff...

You are a lifesaver

Thanks for a great piece of software

Zig