Maximum Stepover / Stepdown and Total Tolerance

[jcnewbie]

I'm trying to understand the direct relation between the total tolerance and maximum stepover / stepdown.. Is there one ?

i.e. If I have a total tolerance of 0.001 what should the stepover = ? Is there a set value that should be placed ?

[ObrienDave]

Total tolerance has nothing to do with stepover/stepdown.
Total tolerance refers to how closely the cutter follows the surface.
For example, if you are cutting the inside of a bowl with a .010 tolerance setting, the CHORDAL error would be .010
Think of it as a parallel surface or curve .010 away from the original.
This would result in a very chunky surface with fewer moves than a smaller tolerance value.
On the other side, a tolerance value of .0001 would result in a very accurate and smooth surface with a lot of moves.
Remember, in Mcam, the tolerance is always applied to the INSIDE of the curve.

[CNC_BOB]

hello OBRIEN
it sounds like you have a handle on how this works and you used the example of a bowl where I would be material safe, my question is If I am cutting a convex shape and I choose .01 surface tolerance for roughing only, is it likely that MCAM will cut across to the shortest distance and violate the finished surface?? this has always confused me
thanks in advance

[ObrienDave]

Yes, you are correct if the total tolerance is equal to, or more than the stock you are leaving for the finish pass.
My rule of thumb is, the total tolerance is 10 to 25 percent of the finish stock.
For example, if you leave .010 for the finish cut, set total tolerance to .001 to .0025
Attached is a screen snippit of my settings for a .005 finish pass.
This is from V9.
Yours might look different.

[lovecnc2003]

thanks

[gorby]

When setting incremental depths to 0,0005 top and 0.0005 other cuts.And total tolarence to 0.0005 on finish contour parametars page,I did not turn noting on total tolerance settig like filter ,my first cut act wierd , tool goes up and down and then next depth is fine .do I have to have filter on for this to surface finih conour work properly.Thank You Im just starting to larn surface tool pasEs.Where else i can find help on surface tool pases Thank You.

[carlosdcerna]

ObreinDave
I am just starting out learing cnc and gcode programing through mastercam. I am having trouble understanding how to leave a polished surface for pet blow moulds on aluminum 7075. Could you please explain the role of the mastercam filter in this process. On the mould i am currently working on right now we did a rough pocket leaving 1mm stock for finishing passes. After that we used a 10mm ball end with .25 stock to leave and finally we used a 5 mm ball end with 0mm stock to leave. The way i was taught was to always turn on the filter and put it on 2:1 and the default .026 mm total tolerance.
Could you please explain the errors in the way we are using the filter.

Thank you

[ObrienDave]

Well, you are not really doing anything wrong.
However, you need to understand what each part of the filter does.

Starting from the top,
The filter ratio modifies the ratio of the filter tolerance and cut tolerance to match the value that is in the total tolerance box.
For example, using your value of .026 and a ratio of 2:1, the filter tolerance works out to be .017333... and the cut tolerance is .008666...
At a 1:1 ratio each value would be .013

Since I have always felt the boxes are out of order, I am going to skip ahead to the cut tolerance box.
Cut tolerance defines how close the cutter follows the actual surface.
It does this by increasing or reducing the number of moves.
The more accurate you want the end result to be, the greater the number of moves.
The less accurate, requires less moves.

Now for the filter tolerance.
If the create arcs in XY or XZ or YZ or any combination thereof, are checked, AND the cuts you are creating are moving parallel to one of those 3 planes, then the filter will attempt to create arcs, in those planes, to help reduce the number of moves.
If your cuts are at an angle to those planes, then the filter tries to reduce the number of moves by reducing accuracy.
This defeats the purpose of trying to produce a ready-to-polish surface.

If I understand your post properly, you want to end up with a surface that is mold-ready-polished.
While this is possible to do, the time it would take would be VERY expensive, especially in 7075 because the Zinc in the alloy is abrasive and even the best
carbide cutter would wear eventually.

I would suggest, reducing your semi-finish stock to .125, reducing the TOTAL tolerance to .0026 and possibly turning off the filter ratio.
This would greatly increase the number of moves and the accuracy of the finished part.
You do not specify what your step-over and step-down values are, so I would suggest finish values of around .25mm to .125mm
My rule-of-thumb is 1/10th to 1/20th the RADIUS of the ball end mill.

This will result in further increasing the size of the posted program.
At this point you will probably have to consider drip-feeding, or DNC, the program to the machine control.

I hope this has helped you.

[carlosdcerna]

I will try this
-12mm dia flat end mill to rough pocket cavity with 1mm stock to leave
filter 2:1 total tolerance .026mm
create arcs all planes

-10mm dia ball end mill to semi-finish the cavity with .125mm stock to leave
filter 2:1 total tolerance .026mm
create arcs all planes

-5mm dia ball end mill to finish cavity with 0mm stock to leave and .05mm stepover
filter 1:1 total tolerance .0026
create arcs all planes


Do you think this is a good way to leave a 7075 aluminum with a ready to polish surface for pet and hdpe blow moulds?

[ObrienDave]

Sorry, I have no experience with any kind of molds.
I do think, however, that these are appropriate values and will give you satisfactory results.
You will probably have to try doing the finish pass in more than one direction,
For example, a finish contour pass will get chunky as the surface angle approaches the XY plane and a parallel pass at say, 0 degrees, will get chunky as the surface angle approaches 90 degrees in the XZ plane.
Same for a 90 degree cut in the YZ plane.