Need Help!- X3 - How to get arc outputs in the X/Z plane?

[colton_m]

Hey guys, I'm stuck!

I am using X3 and have created a simple contour that feeds in the X+ direction and then arc's up in the Z+ direction.

Everything went alright in backplot however, when I post the program it will NOT output arc's in the X/Z plane. It gives me 14 diaganol X,Z moves to create the arc...

I tried turning filtering "ON" and selected "arc's in XZ" but to no avail,

I did some research, but all i could find in the Mastercam help was to check the control definition to esure it defines our machine as capable of performing arc's in multiple planes (X/Y, X/Z, Y/Z).

I was wondering if anyone knows of a way to get the program to post using a G18 command and a simple one line G03 to make my arc?

I programmed the contour this way manually and it works fine in the machine but this was just as a test, later I will need multiple depth cuts so it would be nice if X3 would just post the program with the G18.

I am using the "3 Axis VMC" post processor.

Thanks,
Colton M.

[Superman]

I did some research, but all i could find in the Mastercam help was to check the control definition to esure it defines our machine as capable of performing arc's in multiple planes (X/Y, X/Z, Y/Z).

You are on the right track, Filter must be set to create arcs in the other planes, but it must also be enabled in the control definition file to output arcs, if not enabled, mcam uses the filter value to give point to point code
Op manager settings for filter on for XY, XZ, YZ
settings pull down > control def manager > arcs > turn on "support arcs in ..."

changing the settings in the control def manager is only for this part, to make it permanent, you edit the machine def manager

I was wondering if anyone knows of a way to get the program to post using a G18 command and a simple one line G03 to make my arc?

If you want proper, full arc moves you may have to program to "Tool centre" instead of "Tool tip"......set the tool with warnings and use lead ins and outs larger than the tool radius
Using Tool tip gives a parabola type of toolpath... yes, a point to point output