filtering of toolpaths

[Dave m]

does anyone know the benefits of filtering toolpaths, i know that it creates a smaller program but is it as accurate? and how can i best use the filter for getting an excellent surface finish?

[Zero]

The filter is only as accurate as you set the tolerances to be. I had mine set like this

 

Filter tolerance= .0007

cut tolerance= .0003

 

That should give you an overall tolerance of .001 on the part.

I have since changed it to

Filter tolerance= .0003

Cut tolerance= .00015

which is about .0005 tolerance overall

 

The rule of thumb that I have heard and gone by is that your cut tolerance should be half the filter tolerance and the overall tolerance is a result of the 2.

 

I've had toolpaths that would have been 7 or 8 megs get filtered down to under 1.38 megs( size of space on floppy disk). You want to make sure that your controller (and post processer)can handle arcs in the yz and xz planes when using the filter as well. If they can you might want to change the arccheck in your post to change some of the smaller arcs back into lines or you will get large arcs going in the oposite direction stopping at the same endpoints. If you don't know or don't want to worry about it, in the filter box make sure the create arcs box IS NOT checked. This will make the filter only fiter in xy arcs.

 

Hope this helps

 

[ 04-01-2002, 12:07 PM: Message edited by: Zero ]

[n_tydingco]

Hi Dave,

 

With regard to accuracy, you can change the filter settings by going to SCREEN/CONFIGURE, and choosing the NC SETTINGS tab. Click on the FILTER SETTINGS button and you can set-up whatever parameters you feel will give you the accuracy you want.

 

The default is set up as a minimum arc radius of .005 which has been enough for us to produce parts within our usual tolerance zones.