X8 Surface High Speed (Waterline) - gouges part and weird movements at the machine

[MIKO ELLO]

I don't know if anyone else might be having the same issues.

 

I am using X8 Surface High Speed (waterline)

 

It looks fine on the verfify

 

I post the g code and send it to the machine

 

Fanuc Series Oi MB

 

I run the part and then out of nowhere, the cutter gouges the parts or it does a complete 360' circle when in should just create a corner radius.

 

I have had this problem a long time ago and I had to tinker with the Filter settings to get this to work.

 

Today, No matter what I do. I can turn off the filter or turn it on. The program will just veer off or do these wierd 360' movements and scrap my part out.

 

It's just a simple surfacing of several radii around the edges of the part.

 

Does anyone have any suggestions?

 

I am using IJK's and I have it set to break arcs at quadrants

 

 

 

[MIKO ELLO]

okay,

 

I found some nice information on this site.

 

I changed my values to R's instead of IJK's

 

I changed break quadrants to don't break arcs

 

It seemed to have fixed the problem as far as this program goes

[Rstewart]

Yup, many have had problems from this.  I still use IJK's but also had to change the quadrants myself.

[crazy^millman]

okay,

 

I found some nice information on this site.

 

I changed my values to R's instead of IJK's

 

I changed break quadrants to don't break arcs

 

It seemed to have fixed the problem as far as this program goes

 

 

So it was the machine creating the issues here and not the CAM Software correct?

 

Yes tons of great information on the site and you did what so many fail to do. You took the time and searched for an answer very cool. :unworthy:

[MIKO ELLO]

Yes, It does sound like it's the machine having the issues.

 

The funny thing is that I originally had my post set at R values about 2 years ago.

 

I had this same problem back then.

 

I ended up increasing my min arc length and radius to fix it

 

I have never had a problem until 2 days ago but, its on a newer machine.

 

I will probably change back to IJK's but, I won't activate the break arcs to quadrants and hopefully this will work

[Newbeeee™]

I *think* that IJK is the way to go from previous threads I've read.

R value is an approximation where IJK by nature are precise co-ordinates.

[MIKO ELLO]

Do you know which one I should choose?

 

Delta center to start?

 

or 

 

Delta start to center?

[Guest]

Delta start to Center

[Mjölnir]

I *think* that IJK is the way to go from previous threads I've read.

R value is an approximation where IJK by nature are precise co-ordinates.

 

Using R values causes the control to calculate arc center, start and end points. Rounding error and other situations like where an arc can intersect the next move more than once can lead to unexpected results. Always, without fail, use IJK when the option is available. We have a Sharnoa with a Tiger 5 control that uses R only, but I have only seen it get lost when I programmed it wrong.

[MIKO ELLO]

I changed to IJK's and BAM!! the part crashed. A totally different part and a totally different program.

 

I wonder what other settings I could try??? so frustrating. I don't know what has changed after my update. I just need to tweek my settings somehow

[MIKO ELLO]

I changed my min arc length to .005. It seemed to solve that problem

 

 

Can anyone explain the difference between the "min arc length" and "min arc radius" 

 

Do both apply to the same radius?

[Guest]

Think of min arc length more along the line of chord length

 

The radius is the radius, the length is how long is that radius segment

 

This is what I have set

 

 

 

YMMV

[Maclaw]

MIKO ELLO,

 

I had this problem with "looping" on fanuc OI-MB aswell - for me it's 99,9%

[Maclaw]

Sorry, let's try again (my internet session got busted) :

 

MIKO ELLO,

 

I had this problem with "looping" on fanuc OI-MB aswell - for me it's 99,9% machine tool issue. Take a look at parameter #5008 of your fanuc control (set bit QCR to "1"). This worked for me - but I'm not sure if it's the right solution (maybe I had plain luck...) Another thing is to use AI/APC (G5.1 Q1) - take a look here (read it all ) : http://www.emastercam.com/board/topic/79128-arc-issue-on-fanuc/page-2

 

 

let me know if it worked for you

[Pitka_Guru]

J Paris, that is one nice machine you have. Ron showed me one in Chicago and I'very been talking about it ever since.