Arc Filter Settings

[Brian B 74]

I spent some time looking around the forum but couldn't find the answer I was looking for.

 

For all the mold makers out there - what kind of arc filter/tolerance setting do you use for optimal surface finish?

 

Thanks for the help!

[K2csq7]

Not a mold maker, but I would say these settings are pretty dependent on what your machine can do.... I would go as tight as possible without bogging down the machine. You want the movement to be as smooth as possible (don't want the machine waiting for the control to catch up).

 

Letting others know what machines & controls you have will help you get better answers.

[Mr. Wizzard]

Also not a mold maker, here. Keith is spot on, it depends on your control. High speed look-ahead high-end controls/machines can handle the small linearized arcs and surfacing toolpaths quite well and give you and excellent finish with small tolerances.

 

Myself, however, I go the opposite way. My little Haas machines don't handle look-ahead or small moves, so I open up the tolerance to convert most of the small moves to arcs for a smoother toolpath and "better" finish. I'm better off if my mill can just run through a .500 radius, as opposed to 500 one thou linearized moves. It just stutters and looks choppy.

 

Just depends on your machine/control....

[Teh Bear without Brains kinda idiot]

When I was mold maker I gave total tolerance 0.005 mm and ratio2:1

[Oscar R.]

I've made a few molds in my days but sure won't consider my self a mold maker. With machines and controls that can handle it, I've always used a .0005 total tolorance and at least 2:1 ratio with one way filtering checked on toolpaths that allow it. Also use creat arcs in x,y, and z if you have toolpaths that are moving up and down along walls, like with the blend toolpath.

Seems to me that if you have large sweeping surfaces you can get away with higher #'s on your tolorances using larger diameter tools.

In the old days they used to lap the surfaces on the mold after machining so the finish didn't need to be as good. Then agian they probably had to lap them because they couldn't accomplish the nice finishes you see come out of newer machining centers.

[Guest]

Here's a cap of my typical settings.

 

I just finished some mold programming and the guy was impressed they came off the machine and didn't need any hand work.

[Brian B 74]

Thanks for the response. It is a Roders machining center so it can handle the small lines. Back in the day when I went to MCX school (V9) they taught us to use .0009" with a 2:1 ratio and turn one way on. Now with the fancy filter settings I want to make sure I am doing what most others do.

[Redfire427]

For fine finishing I typically use .0002" with a 1:1 filter with arcs only in the XY plane.

[Chris Rizzo]

.0002 with 2:1 (which is about 30% on the cut tol. slider) and slider to about 80% on the smoothing settings. Working with the smoothing feature I've gotten some really, really good finishes. Processing time goes way, way up too.

 

m2c

[Brian B 74]

Having good luck with a .001" total tolerance. I set NC program length to LONG (no arcs). Surface Quality to Best. Calculation time is normal. Cut tolerance is .0002 and smoothing tolerance is .0008. I was trying the .0002" total tolerance and not only my mcx files were 400mb in size but i couldn't verify them - verify kept bombing out. This seems to be a good balance right now.

 

Thanks for the responses.

[Brian B 74]

I have gotten into some bigger molds and I am back to where my verify keeps bombing out. I have been asking what tolerances you use for finishing. What about roughing? I usually rough to .020" and am using a total tolerance of .005" (calculation time = normal with good surface finish). Do you thing it would be safe to increase the total tolerance to say .010"?

 

Thoughts?

[Thee Rickster ™]

I use total tolerance @ 0.0005" with 1:1 in all axis for everything including 2-d

50% on the slider

 

JP I cant see your, "Here's a cap of my typical settings."??

[huskermcdoogle]

JP I cant see your, "Here's a cap of my typical settings."??

 

Old Post, Probably dropped it out of his photo bucket or whatnot.

[Mic]

It is a Roders machining center so it can handle the small lines.

 

Best output for a Röders is pure line segments. Then the spline interpolation works best. Don't use any smoothing.

 

Röders

 

I would use a finishing tolerance between 0.01 - 0.0005mm. depending on part size and needed surface finish and accuracy.

[Brian B 74]

I use all line segments when running 3D programs. I run lines and arcs when running 2D programs for cutter comp ONLY.

 

I use a total tolerance of .001" (cut tolerance of .0001" and smoothing tolerance of .0009"). I find that when I go to a .0002" or smaller it creates a HUGE MCX file and gives verify trouble verifying. I have started opening up my tolerances for roughing and semi finishing (.005" tolerance for leaving .02" and .002" tolerance for leaving .005"). On our Creative Evolution Machine (10k RPM MAX)

roughing I do a .001" cut tolerance with .002" line/arc tolerance and a .002" smoothing tolerance (.005 total tolerance). For semi finishing I go .002" total tolerance (.0004" cut tolerance with .0008" line/arc tolernace and .0008" smoothing tolerance). I filter in lines and arcs in an X-Y plane only on our Creative. This helps to keep the files size down and verify friendly.