total tolerance / filter ratio

[Rick Henrickson 65]

ok can someone explain in detail the following

 

filter ratio:

1:1

2:1

3:1

custom

 

filter tolerance _______

 

cut tolerance _______

 

one way filtering

 

create arcs is pretty clear

 

minimum arc rad

 

maximum arc rad

 

give discriptions please

[Guest]

cascadeclimber,

 

if you go to the help menu and find filtering toolpaths and display filter dialog box and go to field definitions it will define them for you.

[Rick Henrickson 65]

I know the help menu I kind of wanted to know what the results were and what people are using

[Rick Henrickson 65]

come on there has to be some opinion on this

[wildcat99]

I just cut two similar patterns and with help from this forum learned 2:1 ratio with .0005 total tolerance gives a better finish than 3:1 and .001 total.

 

This was using Surface Finish Contour. One-way filtering seems to help finish, although I can't see much difference in the toolpath when actually cutting. I've tried arcs in all planes, no planes and now sticking with arcs in just the XY plane. Seems to help prevent "stutter-steps" with our router, but I've also made a lot of changes at once, so I don't know which one setting helped the most.

 

Also discovered the spiral limit setting in Finish Contour. This prevents a mark where the stepdowns occur. It is explained pretty well in the help menu and in at least one thread here.

 

My two cents. HTH

[Glenn Bouman]

This article from John Nelson, Haas Applications Manager has some info on tolerances using Mastercam

 

http://www.haascnc.com/solutions_3D.asp#3D

 

It recommends 0.00002" cut tolerance for the perfect finish.

[Keith @ Solid Code Solutions]

How many ZEROs is that!

[Keith @ Solid Code Solutions]

Hey Glenn,

 

Good article, but I guess if you don't have adaptive filtering in the control you have to compensate with something else. I think he must have slipped an extra 0 in there.

[Glenn Bouman]

quote:

---

I think he must have slipped an extra 0 in there.

---

I saw the actual part at a Haas Demo Day a couple of years ago and he had the those settings engraved right into the part.

[wildcat99]

So he engraved an extra zero in the part.

 

Go into 9 or X, pick a surface finish toolpath and try putting in a cut tolerance of 0.00002. It won't allow anything smaller than 0.00005.

[88Matt]

U can set the minimum tolerance in the config settings.

[wildcat99]

Ooops, sorry. Learned something new again today.

[Jaz]

My take on what the filters do. The 'Cut tolerance' is how close MasterCam follows the surface when it generates the path. This value greatly affects processing time, i.e. the smaller the number, the harder MC has to work at it. The 'Filter tolerence' is applied to the paths that MC generates and atempts to turn lots of point-to-point code into arcs and long straights. This value greatly affects the length of your NC file. Both numbers affect the accuracy of your finished surface to different degrees, how much each affects the final product has a lot to with the shape of your surface. I usually drive finish paths with .0002" cut tolerance at 3:1 ratio for a total tolerance of .0008". This is usually adequate. Roughing paths I use .001 + .003 for .004 total. HTH