parallel surface question

[mike.b]

is it possible somehow to get rid of the retracts that happen at the beginning and end of a parallel surface finish toolpath? for example if you were surfacing a circular planar surface the tool retracts when the angle to move to the next toolpath gets more extreme.

this is drivin me nuts!

[Christian Raebild]

It is the gap settings that govern when those retracts occur.

 

At the top of the gap settings dialog, you can set the maximum distance where the tool will not retract, either as an absolute distance or as a percentage of the stepover. If you set that distance high enough, then the tool will not retract between the passes.

 

You will of course also have to set the behaviour on motion < gap correctly, often either "broken" or "follow surface" works well in such situations. What needs to be set there depends on the part geometry, though.

[richardtraver]

increase your gap settings. use distance and if you make it .5 - 1. and the tool should never retract

[steve f]

Here's a fairly easy fix for the situation you're talking about. Go into the "Gap Settings" window in the third toolpath parameters page of the surface finish operation. Increase the "Gap size" distance or percentage until the retracts are eliminated. Use this feature with a little caution if the part you are toolpathing contains many and/or small complex surfaces because there is a danger of gouging if surfaces were missed when selecting them as check.

 

ex: two surfaces are seperated by a tall standing rib and the "Gap size" specified to eliminate many retracts is larger than the distance between the two surfaces being cut. If the surfaces that define the rib are not selected as check, Mcam will not know to retract between cutting the two surfaces and may create a straight line feed motion to begin cutting the second surface gouging the rib in the process.

 

HTH

 

steve

[steve f]

looks like everyone beat me too it,

 

steve

[mike.b]

i love this forum. i was playing with gap settings but didnt think about the distance ..duhh thanks guys

[Teh Bear without Brains kinda idiot]

~~~~~~~~~~~~~

surfacing a circular planar surface

~~~~~~~~~~~~~~~

If I understand right your geometry ,I would prefer surface->contour toolpath .

 

JM2C

[John Q]

Will this work on surface pocket also

I tried with no success

[Thad]

John Q,

 

Surface pocket and surface parallel function differently. With pocketing, you should only be getting retract moves in 2 different circumstances. 1 is when the tool can't get to where it needs to, because of containment boundaries for example. Imagine cutting surfaces that form an upside down "V." Since the pocketing cycle does a planar cut, it will cut on one side of the V, retract, and cut the other side of the V for each depth cut. Select "Optimize cut order" to eliminate this. That will make it cut one side completely, then the other.

 

The second reason for retract is when the tool finishes making a complete pass at any given depth cut. You can't do much about that (safely, that is).

 

I hope I didn't confuse the issue.

 

Thad