3d surfacing settings

[K2csq7]

I was looking for answers to how the filters affect accuracy of the posted code. But it seems no one wants to comment on that. The documentation mastercam gives refers to the shape of the part when talking about when and what to use for filters. That's why I posted an example of the part. Thanks for those who did comment something useful. Hopefully some else can chime in with some settings that are proven to work

You are not asking a question with a black and white answer. We can't say ".005 total, with 76.2% cut tol..." or whatever.

From this thread you should have a good understanding on what affects what. Getting the "perfect mix" for your machine, your control, with your workholding, your tooling, and your material, will only be attained by trial and error on your machine, your control, with your workholding, and your tooling, cutting your material.

 

Best of luck FTI. Let us know what works out!

[FTI2007]

I get what you guys are saying but I'm not sure if I'm wording my question correctly. How far can I open up the filter settings before I have to worry about the code starts to deviate from the model. That should not be effected by the memory size of machine, setup , or tooling used. I don't have the luxury of having time to play with settings on 1 off parts. Thanks anyways

[crazy^millman]

I don't have the luxury of having time to play with settings on 1 off parts.

 

That pretty much tells me I go for what gets the job done. It is what is it and if someone wants it faster then I tell them to take 100% responsibility for the part and show me a faster way. Getting it dialed in take trial and error and with 1 off parts I always did what I knew was 100% safe. Time is what it is.

[djstedman]

As to your question I would say you can safely assume based on the comments from Colin that whatever your total tolerance is the amount your toolpath will deviate from nominal, so the total tolerance should reflect the amount that you are willing to allow the toolpath to deviate from nominal, keep in mind that's still only the amount your toolpath might vary.. it doesn't include any deviation caused by stresses of machining itself..

[LaszloK]

I have experimented with different filter settings for finishing large mold blocks using the "High Speed Scallop" toolpath on machines with very little look ahaead. I know your pain. As you say, roughing is not the problem, feedrates slowing way down to make all those .001-.002 linear moves in the finish toolpath is frustrating. File size, toolpath regeneration, and time to verify are additional problems. We also need tight tolerances and can not back off in the filter setting too much. I have reduced finish machining time by opening up the scallop height setting a bit. We used to use .00003 scallop height in order to get good surface finishes. Using a scallop height of .00006 instead still provides a pretty good finish and a shorter run time but does not eliminate the problem with feed rates going down. I am currently experimenting with different toolpaths. The combination of "Horizontal Area" and "Waterline" toolpaths are showing merrit in the mold cavities we machine. Just run the Horizontal Areas toolpath first then the Waterline.

[FTI2007]

Thanks guys,

 

Laszlok, most of what we do have very little flat areas. most of it seems to have 1/2 degree or more that we need to match so horizontal area doesnt do much go there. but i do use it where I can. I havent had alot of luck useing waterline on parts like this but I havent tried for awhile either.

[shazam/TPP]

you said previously on the filter page that you only click the xy for arcs, why not also click xz and yz? 3d contour surface should help.

i have my filter settings set to:

total tolerance=.0005-.001

cut tolerance = 25%

line/arc tol = 75%

activate xy, xz, yz also depends if i want acrs generated on those planes

rarely use the smoothing setting

 

ps what size ball mill do you use for finishing in your example?

[mike93]

if you add tool path radis of .005-.01 for scallops it helps alot, small zig zags on the edge of a part will slow a mill with look ahead and high speed down to a crawl, older controls it can be really bad

[MotorCityMinion]

"I was looking for answers to how the filters affect accuracy of the posted code. But it seems no one wants to comment on that.'

 

O.K. I',m in. Filters of any type, on anything, arc or smoothing, always effect the code, and quite possibly in a dirty fashion. Set the tolerance to .00005. no arcs of any type, and you'll get as close as possible. Don't have room for code? That's a separate issue. Machine worn out? HA, everything else is mute.

 

"That pretty much tells me I go for what gets the job done. It is what is it and if someone wants it faster then I tell them to take 100% responsibility for the part and show me a faster way. Getting it dialed in take trial and error and with 1 off parts I always did what I knew was 100% safe. Time is what it is."

 

No BS here as I couldn't agree more.

[FTI2007]

you said previously on the filter page that you only click the xy for arcs, why not also click xz and yz? 3d contour surface should help.

i have my filter settings set to:

total tolerance=.0005-.001

cut tolerance = 25%

line/arc tol = 75%

activate xy, xz, yz also depends if i want acrs generated on those planes

rarely use the smoothing setting

 

ps what size ball mill do you use for finishing in your example?

 

 

Im using a 1.25 ball to do majority and step down in sizie to get corners/leftover areas

 

Im not sure why I didnt use arcs in al lplanes. im goin to try that now.

 

 

if you add tool path radis of .005-.01 for scallops it helps alot, small zig zags on the edge of a part will slow a mill with look ahead and high speed down to a crawl, older controls it can be really bad

 

Im not sure I understand this. Where/How is this done?

 

 

 

 

 

Machine is not wore out. It just does not have much memory so we DNC to it and it does not have high speed look ahead. its about a 13 year old fanuc controller.

[FTI2007]

Just trying to make the most of what we have.

[crazy^millman]

Look here for toolpath fillet:

 

 

HTH

[FTI2007]

cool thanks. ill have to try that to. So far we are making lots of progress running a .001 total tolerance. with a cut tolerance of 50% cut tolerance and 25% line/arc and smoothing. At least double actual feed rates. Fingers crossed

[crazy^millman]

Awesome keep us posted sounds like you are getting it dialed in.

[MrFish]

I have experimented with different filter settings for finishing large mold blocks using the "High Speed Scallop" toolpath on machines with very little look ahaead. I know your pain. As you say, roughing is not the problem, feedrates slowing way down to make all those .001-.002 linear moves in the finish toolpath is frustrating. File size, toolpath regeneration, and time to verify are additional problems. We also need tight tolerances and can not back off in the filter setting too much. I have reduced finish machining time by opening up the scallop height setting a bit. We used to use .00003 scallop height in order to get good surface finishes. Using a scallop height of .00006 instead still provides a pretty good finish and a shorter run time but does not eliminate the problem with feed rates going down. I am currently experimenting with different toolpaths. The combination of "Horizontal Area" and "Waterline" toolpaths are showing merrit in the mold cavities we machine. Just run the Horizontal Areas toolpath first then the Waterline.

 

Whoa , that's some fine tolerances and must take a lot of power and time to crunch the numbers !!

We never go below 0.0035 mm total tolerance for our mould work or it just takes too long to generate the tool paths.

[LaszloK]

It does take some processing time but we do verey little mold polishing.

[shazam/TPP]

also try using the high speed raster. the beauty of the high speed surface toolpaths is once you have selected your surfaces you can switch to a different path style without having to reselect your surfaces. ie high speed scallop then switch to high speed raster. the high speed raster produced a much smaller file (65% less) than the high speed scallop using the same tool and filter settings and scallop height (.0006)

 

edit: plus a shorter cycle time

[LaszloK]

High speed raster is a good toolpath when you do not have verticle or near verticle side walls.

[shazam/TPP]

^^^ true that

[Müřlıń®]

I was looking for answers to how the filters affect accuracy of the posted code. But it seems no one wants to comment on that. The documentation mastercam gives refers to the shape of the part when talking about when and what to use for filters. That's why I posted an example of the part. Thanks for those who did comment something useful. Hopefully some else can chime in with some settings that are proven to work

 

Filter settings affect code output 10 to 1.

 

But if your post is not dialed in you could have gouges that do not show up in verify. Point to point linear is the most foolproof way to post it but the code is monstrous...

 

I looked at your part and if I was to machine it, there would be multiple windows..several different toolpaths would be used.....waterline, scallop and raster, horizontal and possibly pencil.

 

 

 

.