Finish pass?

[budpage]

Still trying to understand a simple finish pass process. Can I add an additional mop and specify a negative stepover number of, say, .005 ? Will this work or is there a smarter way? I've read most all of the CamBam postings and found this subject only 3 times since 2002. This tells me that most everyone must know how to do this but I'm not there yet. Thanks...

[cornbinder23]

I think I asked about this once but basically IIRC there was not a "FinishPassButton" in the drop down menus, would be nice if CamBam could incorporate that, but here is how I do it, may not be right but it works for me.

First, You can offset the polyline you are creating a MOP for, and machine that first and then create another MOP with the original polyline
So for instance I am cutting a 2" pocket .5" deep I would draw the original polyline then offset it inside about .001" then make a pocketing MOP for it and machine the pocket first, then come back to the original polyline and make a contouring MOP on the inside of the pocket and cut that at full depth of the pocket and it gives you a finish pass on the wall of the pocket, if you want to finish pass the bottom of the pocket you would have to hold back on your depth the amount you want for a finish pass, and make the second op a pocket at full depth and you will have a finish pass for the pocket.

Second, another thing I do is fudge the tool diameter number to reflect the amount of material I want to leave for a finish pass.
So, using the example 2" pocket above,using a .25" endmill I would select the 2" dia polyline and start a pocketing MOP, setting the cutter dia to .24
then select the same polyine and create a contour or profile depending on how you want to finish cut and set the cutter dia to .25 and you will have a finish pass

So thats the long and short of how I get finish passes using CamBam, I really like the software and have really never had any issues with it, hopefully they can work this out in development,and get the experimental turn functions nailed down but there are alot of people using and supporting this software.


JTCUSTOMS

[10bulls]

I think Roughing Clearance is the property you are looking for.

Entering a small, positive value here will leave that much stock remaining after the machining operation.

You can then follow this with another 'finishing' operation with the roughing clearance set to zero to clear off the remaining stock.

Roughing clearance will also accept a negative value which will over cut the stock by this amount. This is very useful when making parts that need to fit inside other parts, like inlays for example.

Turning View - Show cut widths can make it easier to see the effect of using roughing clearances.

CAM styles are also another handy feature for this sort of thing.
You could create a 'roughing' style, with roughing clearance, aggressive cuts, fast feedrate etc, and also a 'finishing' style, with zero roughing clearance, slow feeds etc.

It should then be a case of selecting your drawing objects, inserting a machining operation and setting it's style to 'roughing'; inserting a second operation and setting this ones style to 'finish'.