3d surfacing settings

[FTI2007]

I am trying to find a way to produce less code in my 3d surfacing programs. I use surface high speed scallop for alot of the parts I make. The machine we run the larger parts through does not have look ahead and really bogs down running some of the parts. sometimes down to only a couple inches a minute. I do filter the code but maybe there is somthing Im missing or doing wrong. any help would be great. Thanks

[Tyler Robertson]

Does your machine support subprograms? Do you have DNC already?

[K2csq7]

If I leave .010 stock on the walls, I'd set my "Total Tolerance" to .008 (gives me a .002 cushion), check the box for "line/arc filter settings", also check the box for "create arcs" in the appropriate plane. Then slide the slider all the way to the right. Small cut tolerance, large line/arc tolerance.... that will give you the smallest amount of code.

[brandon b]

Filter filter filter

[GoetzInd]

Yeah, what kind of filter settings are you using? Maybe post a screen shot.

 

Mike

[djstedman]

K2csq7, I could be wrong but as I understand the documentation, the 'cut tolerance' is the amount it will actually influence the cut surface.. so for example if you had .01 stock left on walls.. your 'cut tolerance' could be up to .008 (well actually .0099 if you were that crazy)

 

Anyhow.. the line arc tolerance is the amount of tolerance that your allowing Mastercam to use in its algorithm to determine the most efficient way to modify the points in the toolpath to come up with smaller code..

 

Its totally possible im not understanding it right from the documentation but I thought that's what it meant..

[K2csq7]

djstedman,

It's all a guessing game to me... I go by the toolpath size (in the ops manager when the toolpath is expanded). Sliding that slider to the right makes the toolpath size smaller...

[Gary]

Use contour ect? scallop makes for big code. Easy/fast to program makes for larger files almost always.

[FTI2007]

Im not sure how to take a screen shot. All I do Know is that the I need accurate parts with a good finish. I usually use a total tolerance of .0005 on the filter page and leave the sliders in there default location which is a cut tolerance of 90.2% (.000451) line/arc tolerance of 4.8% (.000024) and smoothing tolerance of 5.% (.000025). I have create arcs in XY checked with a minum arc radius of .005 and max arc radius of 100. use max value for both is checked. smoothing settings is checked with shift points randomly and minimize number of points. I think the hole filter page should have more info to go with it on how and when to use what setttings. everything I make is custom 1 off parts and I dont get time to experiment much settings. I hope this helps explain what im currently doing. Answers like filter filter filter do not do me any good without some direction. Thanks

[K2csq7]

You can't have your cake and eat it too!!!

Use roughing paths for roughing, then finish.

[djstedman]

Sounds like you would see your toolpaths shrink a lot if you were to try what K2csq7 mentioned earlier.. allocate more of your total tolerance to arc/filter tolerance.. generally splitting it about 65% to arc/filter and 35% to cut has seemed like it has yielded the best results for me in most situations.. with much smaller (usally about 4 times smaller) code.. and pretty much equivelant accuracy as unfiltered code

 

Also like he says.. on roughing paths.. leave more stock then open those tolerances up wide to really reduce code and have the ability to move faster since you have far less short linear moves.. ie leave like .01 or .015 and open up total tolerance to like 80% of whatever amount of stock you leave..

 

On finishing paths depending on the shape your cutting and the path your using you might just be stuck with filtering not doing you a lot of good no matter what.. as the documentation in the filtering section mentions "In 3D surface machining, line/arc filtering works best for “kinematic” surfaces such as planes, cylinders, cones, and spheres."

additionally they mention .. "Line/arc filtering may NOT be suitable for sculptural (free form) surfaces."

 

That said .. its worth trying the guidelines above on your finishing paths as well .. and seeing how it works..

[FTI2007]

Of course I rough the surface down leaving .020 for finishing. Im not sure where that roughing comment came from K2cq7. These blocks are p20 that start out over 1500lbs and finsh at 2-300lbs. AJX feed mills love these. I was thinking total tolerance was like the finished machined surface compared to the cad. So that is why I have it set to .0005. If I open it up to .01 like he says with his settings I do see wthere if you move the slider the cut tolerance stays at .0005. ...So my acuracy should stay the same Correct?? thanks again for the comments.

[crazy^millman]

Have you looked at the HST toolpaths with Full Carbide Endmills to rough that beast?

[djstedman]

I just went back and found a post that I remembered that Colin from CNC Software had made.. where he explained this better.. now that I have re-read it its a bit clearer to me.. basically sounds like from what he said both the cut tolerance and line arc tolerance play a role in the accuracy of the end result..

 

This is what Colin from CNC Software said in another post a while back about line/arc tolerance vs. cut tolerance ..

 

 

I've covered the Filter settings numerous times on here. If you do a search, you'll find lots of information.

 

The ratio you are seeing is the "Filter Tolerance" to "Cut tolerance" ratio.

 

When you create a toolpath, the first thing that happens is the entire toolpath is linearized. Then the toolpath uses the "cut tolerance" filter to remove moves from the path that are smaller than your tolerance (basically we try and fit a single line to a section of line segments, if it is within the given tolerance).

 

Then the "Arc Filter" runs on the toolpath. This attempts to fit Arcs to the toolpath, within a given tolerance.

 

So the ratio is the split of the "Total tolerance" between the "cut tolerance" and the "arc filter" tolerance.

 

Hope that helps,

 

Colin

[FTI2007]

So If set the total tolerance to .010 and slide the bar so my cut tolerance is .0005 what will my end result be? Will it be acureate to could it be .005-.009 off from the cad?? Thats where I get confused I guess. I dont have a way of measureing the final result.

[FTI2007]

I have played alittle with the HST toolpaths for roughing but have not had much luck in steel. I think mostly because we only have general purpose Garr. Roughing is not the problem. just trying to speed up finishing.

[FTI2007]

I just found this posted by colin also....... Maybe this is where I came up with a tight totol tolerance. Unless Im reading it wrong...

 

 

(Copied and pasted)

 

No, I'm not saying you need to never use Hybrid. I'm saying you should set the Horizontal Arcs setting to zero for the linking parameters. That should prevent the issue from showing up in X6. This issue has been fixed in X7, and all linking moves are now gouge checked against the drive and check surfaces. (BTW, X7 also now supports check surfaces for these HST toolpaths)

 

I prefer the 2:1 ratio when setting my filter, as it keeps the path more accurate, while allowing better arc filtering. You can do a search on this forum for information about the toolpath filter and find some great info. There are basically two filters that run when you make a toolpath. First, the entire path is linearized, using the 'cut tolerance'. This is a bi-lateral tolerance that determines the initial accuracy of your toolpath. After the cut tolerance filter runs, then the Arc Filter is run. This filter will fit an arc to the linear segments, within the given tolerance.

 

My basic starting parameters for Total Tolerance is 10% of the Stock to Leave value. So if you are leaving .100 of stock on your surfaces, then using .009 for the total tolerance is a good value. The larger the tolerance, the more filtered your code is.

 

For finishing, I like to use a value of .0003 for most contouring/surfacing. The only exception for me is very tight tolerance cuts. In that case I will go down to .00001 or less for my total tolerance, basically whatever the lowest tolerance the dialog will let me enter.

 

The ratios you choose just take the total tolerance and divide that value up between the two different filters according to the ratio you select or enter.

 

Hope that helps,

 

Colin

[mkd]

one simple thing to strive for that can have a HUGE effect on file size is the direction you toolpaths run over your parts.

by selecting the right toolpath (contour, scallop, flowline, parallel etc) you can reduce file size by having the algorithm take advantage of straight cuts. often times a 45° raster is going to be larger than a 0° or 90° raster.

[FTI2007]

Every toolpath has its place. I just want to focus on the filter settings to reduce code but still get an acurate part. I would think everyone would want a good part with least amount of code possible. Like in previous versions when you picked rough better best on the filter page. To me that makes more sense.

[Aaron Eberhard]

Put up a part, it sounds like a fun challenge for people

 

"Here's a raster part, tweak the tolerances while keeping the overall surface tolerance at X, and post how small you got the NCI file."

[FTI2007]

Here is one example of the part .....P20 Steel

EXAMPLE.MCX-7

[FTI2007]

So anyone have some good filter and smoothing settings for this part? Looking for a good finish and acurate part with minimal code useing surface high speed scallop. I was going to try a total tolerance of .005 with a cut tolerance of .00025, line/arc tolerance of .0007 and smoothing of .004.

[djstedman]

If you posted the file with some toolpaths on it i'm sure people would be happy to look at the filter settings ..

 

I don't think most people have the time to spare to toolpath the entire thing as well ..

[FTI2007]

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

[crazy^millman]

Taking your part and using the opticore toolpath with filter settings turned up I see about a 1/3 size in the file. With no filter settings I see a 11611.K file. With Filter setting truned up I see 4112.K file size. Accuraccy should be a concern, but what will run best on the machine and give you the most efficient way to run the part will have so many different factors hard to know.

 

#1 Do you have enough memory to put big programs on the machine?

#2 Does your machine have Look Ahead? HSS filtering capabilities?

#3 Does your machine have problems with small or big arcs?

#4 Does your machine handle looser tolerances well and in your tests what has proven to be the sweet spot?

#5 Do you take the time and try some 2D stuff and mix it with the 3D HST toolpaths?

#99 And yes we could break it down that finite.