[Claude Boudreau]

Is there a way of smoothing my tool travel , it`s stopping an instant between entities causing a somewhat rough movement.

[Kiwi]

Sounds like a controller setting, not the code.
Check your controller manual on Look-Ahead.

[moldmker]

If your feedrate is set too high it will make for jerky movements.

The threshold is dependent on the vintage/power of the control. My older Fanuc can't be pushed more than 30 IPM on 3-D paths. Same path will run on newer Haas with high speed machining package at over 100 IPM.

Also, some older controls have a mode called "In position checking" which causes a slight lag between blocks while checking position.
On my Fanuc it's enabled with G61

moldmker

[Khalid]

if using Mach3, enable CV mode in config> state or put G-64 at the top of G-code

[ImanCarrot]

Just a thought- is your machine balanced on the floor?

ie: If there's four footpads are they all in contact with the floor... perhaps one isn't and the inertia of the machine is causing toppling?

Definately worth checking and appologies if this don't help, but I've seen this before on an old machine.

[ImanCarrot]

Double post- sorry.

[Vega Bill]

There are several things that can cause jerky motion on CNC’s. The first is as noted in earlier posts is the look ahead (G08 on some CNC’s) and corner rounding settings.

There are several other issues that arise when machining complex surfaces that many CAD systems ignore and most people are unaware of. The first of witch is the Block Processing Rate (BPR) of the CNC. This is the speed that the CNC can digest a single line of the program. Since the early 80’s the magic number was about 8 mili-seconds. In today’s high speed systems, the best we have benchmarked is 1 mili-second and that is for a typical 3 axis application (5 axes about 1.8 mili-seconds).

The problem this creates is that CNC’s react differently to densely populated data areas when the feedrates are higher than the point spacing. For example if you had a gentle swept surface where the data points were evenly distributed every 0.01 inch and your CNC had a (BPR) of 5 mili-seconds, the fastest feedrate that could be achieved without jack hammering would be 120 IPM ( 60/0.005 x 0.01).

The real problem begins when you try use high speed machining practices with feedrates above 100 IPM and point distribution ranging from 0.025 inch in the straight areas and 0.001 in the curved areas. Most all CNC’s will react poorly to these circumstances and some will become down right violent. Banging, slamming, jerking, and breaking cutters. The second part of this problem is that it is difficult at best to determine where the CNC will have problems digesting the data without the aid of surface analyzer. So most people just turn the feedrate down.

We have been working on Feedrate Optimization for over 5 years and have showed dramatic improvement in cycle time, surface quality, and cutter life. Some of our customers have reported up to a 300% increase in throughput with a better finish.

The Feedrate Optimization takes care of all the look-ahead and pre-digests the program for the CNC. It embeds acceleration and deceleration points into the program based on Motion Dynamics. The Motion Dynamics include the G forces applied to the machine, the BPR of the CNC, Baud Rate detection (for drip feeding), and contour recognition.

We have a BPR test file available if anybody has an interest please PM me.

If you would like to try the Feedrate Optimization, there is a fully functional demo available at www.vegacnc.com (it is part of the VEGA DATA-View package)

[shey_med]

I had same experience as u felt.first of all Check your parallel port outputs are working properly.

[Machineit]

I had same experience as u felt.first of all Check your parallel port outputs are working properly.

Welcome to the forum, but this post is 4 years old. I've done it too!

Cheers--Mike

[shey_med]

Hi ,i didnt see the post date.. sorry for the date ignorance. Any how could u share with me how u solve the problem.

[Claude Boudreau]

Hi ,i didnt see the post date.. sorry for the date ignorance. Any how could u share with me how u solve the problem.

Its been a while but I think it had to do with settings of Constant Velocity.

Check this link http://www.cnczone.com/forums/mach_s...on+%28solution

hope this help (if you got Mach3 )