im doing some surface ballmill work on a die and need to find out how to make mastercam stop generating a million lines of code when it cuts an arc over and over. is there a switch somewhere to force output of arcs instead of a million tiny straight lines?
check this out
Why is My code size it wayy too big?
Thanks, but increasing the tolerance in the parameters window
is only making the straight lines longer. i tried increasing up to .006
im cutting in xz plane , does that matter?
Inside the tolerance button there is a box to check that makes arks in yx yz xz. turn that on and set tolerance to 3:1
WANNA GO FASTER
Depends on the Mastercam Version being usedInside the tolerance button there is a box to check that makes arks in yx yz xz. turn that on
"Allow Arcs" is in the FILTER area only
this is generally for surfacingand set tolerance to 3:1
Anything other than OFF will allow arcs to be posted
To get any post to output arcs, there are 2 areas to be checked
1- in the operation parameter FILTER area, where you can actually set it ON or OFF to suit any situation.
Normally you would set these fields to ON in the operation defaults, so you don't have to check it everytime you create an operation
2- in the CONTROL definition file, under ARCS, allow arcs for the various plane combinations ie XY, XZ, YZ must all be checked ON to recognise the settings within #1, and then it allows arcs to be in your NC code
Now if you set #1 areas to be ON, but they are NOT SWITCHED ON in the control ( #2 ), you will only get point to point code, not arcs.
ANY SPLINE will give point to point code
ANY ARC NOT laying completly perpendicular to the tool plane WILL GIVE point to point code, as it is considered an elipse ( which is a type of spline )
NOTE 2 ---
ie a ballnose cutting inside 1/2 a cylinder
Arcs in planes other than XY, a toolpath that uses the tooltip as the calculation point will not remain a constant distance away from radial geometry, it will generate longer programs than expected
using the center of tool ball is the only point that stays a constant distance from geometry. Caution must be shown if programming to this method as well as setting the tool on the machine
is this only for the surfacing tool paths? Im having trouble with simple roughing passes being too big
when i went into the control manager and set those things you said
suddenly i've lost the r's in my arcs. now on delta, and they wont go back
why is this?
OK, it is now reading your control settings
under that area ( Arcs ) in the CONTROL file is the "Arc center type" set it to "Signed radius" ( any arcs bigger than 180° of sweep has a minus sign inserted )
under that again and set the break arcs at 180° ( you should have no arcs output with a minus sign )
( do this for each of the planes )- this breaks the circles ( or large arcs ) into 2 pieces, this allows for slighty faster feedrates on some of the older machines that may distort radial movement when feeds are toooo fast.
Set the Helix support to "Only in XY plane" - this is for the ramping in action on some strategies.