Another Smooth Arc question...

[SuperDave]

... Dave has been far too quite lately...

I have an issue with smooth arcs and circles. I export a .dfx file and open in Aspire. The arcs were made with a three point arc command. The file opens in Aspire fine. In node edit, there are three arc point as you would expect.

However, when my machine runs (Techno Isel 4896 Plus Servo system with less than 20 hours run time) it makes choppy, rough marks all along the tool-path. It makes no difference what size the arc is or if it's an exterior or interior. The image is for a 10" arc with three points and the finish is as choppy as can be.

I slowed the feed to below IPM and increased to 300 IPM and get the same quality. The 1600 pound router jerks like it is trying to chop wood with a dull axe when it gets to an arc.

It's always nice to see someone's home brewed CNC router run smoother than your commercial one... then have a client ask about the rough cuts....

[GripUs]

Hi Dave,
I have a Techno-Isel as well and had the same problem until I changed to the "Techni-Isel ATC Arc (inch)" post processor. I don't know which one you are using but if you are using the other one, you might try this one.

I don't know if it would make any difference but you might also take a look at your acceleration.

Of course, if all else fails, call Bob at Techno support and he will have you fixed in no time.

Regards,

Joe

[SuperDave]

Joe,

Good idea. I will test that PP over the weekend and report back. I was using the Techno-Isel ATC (inch).

Glad to meet another Techno user... need someone to bounce things off of from time to time.

I am looking to upgrade my machine to an ATC without paying the full-monte through the dealer, so fixing this issue before hand will be a blessing!

D

[kilrabit]

If this does not help much choose an arc you are having trouble with and choose the "fit curves to the selected vectors" icon, when using someone else's drawing this has happened to me before.

[gravirozo]

hello dave

of your description, without i can see any settings, or g code... i could assume two thing..

one, the acceleration decceleration might different on x and y axis...

your output contain short segments, and your machine stop on all nodes... ie controllerprograms can be configured on two way, in one option it will stop on all node...in other option will be used the so called cv, continous velocity... where will be precalculated the velocity between segments, pending on the angle they are laying... in this option also you have settings for "buffersize" you can set for your computer-processor... if you can set larger then your program calculate more segment in advance, does mean in case short segment it can be even hundred of segments...

but also a point joe gave you, and i think that the best call techo and they give you support... because a servo could not "jerking" on this toolpath you posted, even with 300 ipm...

your machine has german made elements... i think among the best... i used isel controlprogram in the late 90's that was run under dos and the screenshot was blue and green blocks... in that time it was very modern...

and homemade machines has factorymade rails and ballscrews.... so they could do real good output...


thanks
viktor

[SuperDave]

Hi Dave,
I have a Techno-Isel as well and had the same problem until I changed to the "Techni-Isel ATC Arc (inch)" post processor. I don't know which one you are using but if you are using the other one, you might try this one.

I don't know if it would make any difference but you might also take a look at your acceleration.

Of course, if all else fails, call Bob at Techno support and he will have you fixed in no time.

Regards,

Joe

Joe,

I just tested the PP you suggested and it worked to perfection! Nice smooth Arcs. I did have to re-run the file and slow the feed from 300IPM to 150IPM, as the bottom of the hexagon pocket looked like it was chiseled out by hand! I think the 300IPM feed with .015 step-over, was a bit fast for the .125 Endmill... I reset the pocket depth and got a really nice finish.

There was one element that threw me for a loop as the I ran the file... The spindle went to the "Z" start position, went to depth and then stayed there as the -Z reading compiled from .000 to the -.125 cutting depth before starting the tool-path for the first pocket. I ran a total of seven different pockets and the first one (octagon) was the only one to go through this routine... maybe it was because it was an octagon pocket?

I sure wish the Techno Isel control software had a better and more in-depth reference manual.... but, hey! I get nice Arcs and inner/outer profiles now!!

[SuperDave]

hello dave

of your description, without i can see any settings, or g code... i could assume two thing..

one, the acceleration decceleration might different on x and y axis...

your output contain short segments, and your machine stop on all nodes... ie controllerprograms can be configured on two way, in one option it will stop on all node...in other option will be used the so called cv, continous velocity... where will be precalculated the velocity between segments, pending on the angle they are laying... in this option also you have settings for "buffersize" you can set for your computer-processor... if you can set larger then your program calculate more segment in advance, does mean in case short segment it can be even hundred of segments...

thanks
viktor

Hi Viktor,

I checked and the Acceleration was set to 20 on all axis. I also have it set for Continuous rather than Step. I used the Techno PP that Joe suggested and got really nice Arcs!

The only thing I could not find, was a setting for the buffer or "Look Ahead"... so I assume the Techno control software, being a Windows based program, uses Windows setting rather than a setting in the control software... but that's just a guess... I sure wish Techno would create a more in-depth reference manual....

Thanks for the suggestions!