Filter settings

[Lars Christensen]

Hi guy's,

 

I have been reading the help collum in Mcam, and did a quick search here, but I do not allways trust my ability to understand english.

 

I can understand the point of eliminat small line segments if you are working with a surface modul(what I have onely done once, and I actelly believe it asked me for a tolerance)but if you are working with 2D should you use it? if I understand the purpose of filter then you wouldent.

 

Thanks

Lars

"I hate when I dont understand things"

[Fig sign]

2d contour may consist of splines or and lines/arcs of 0.001 length .

You will get without filtering so loooooooooooooooooooooooooooooooong code !

 

Iskander teh always use filtering

[Fig sign]

Navot Eng !

 

You were looking over this thread !

If you are reading this post why you are not stop lurking here and start to write from time to time ?

 

Iskander omer Shalom !

 

[ 10-14-2003, 02:11 PM: Message edited by: plasttav ]

[Müřlıń®]

Lars, choosing arc filters will put G02 and G03 blocks in your NC file.

 

If you are doing a lot of corners on your part, sometimes turning of the arc filters will allow your control to be smoother in the corners.

Thus you will be able to run at greater feeds without servo studder.

 

You will really notice the change when you go to 3-d.

 

Turning on the arc filters will turn a 3000 KB file into a 300 KB file.

 

This will allow you to run Scallops at 200 IPM

that you couild only get to run at 75 IPM before.

 

 

Murlin

[crazy^millman]

Filter all the way seen it take 50 mb files and turn them into 8mb files. It make a smoother looking parts and doesn't make it look so faceted on the surfaces or in the curves. Also make sure you post is set up output arc move for your machine correctly.

 

Crazy Millman

[Müřlıń®]

quote:

---

Also make sure you post is set up output arc move for your machine correctly.

---

this could be easier said than done....heh

 

 

Murlin

[Lars Christensen]

The filter box will be checked from now on, thanks for making me understand what this feature does, I can now see have it could make my life easyer.

 

Any hint on what I need to check in my post? to see that I am running filter correct?

 

Thanks guy's

 

Lars

[Müřlıń®]

You just need to be familiar with what your control requirements are for circular blocks.

 

Post a file with the arc filter turned on and either do a dry run or observe the code.

 

It might work fine the way it is.

 

Murlin

[HevyMetl]

One thing I have to be careful of in filtering surfaces created by parabolic spine equations is that if you don't set your filter small enough with a fine total tolerance you get small gouges. I acutually make the surface rougher because two side by side passes will out put slightly different radii causing small gouges in my electrodes. I try to run a .0003 total tol with with a .0007 filter with .005 min arcs when I need to decrease a file size. By the way my biggest parts are 1.5" by 1.5"

 

Has anybody else expiremented with these setting for best results?

[foolsh]

yes i too find some streaking lines on my copper electrode after using filtering and sometimes the workpiece got damaged from gouging!

[crazy^millman]

Glad it helped Lars but keep what has been said cuase it can cause the problem listed. I got a part cruching toolpaths right now figure it will take 14 hours to cruch the .002 stepover on the finish scallop toolpath I am doing right now. I think it will be upwards of 70 mb toolpath with the filter on so you can imagine the fun.

 

Crazy Millman skippy do da skippy pe day my on my what a wonderful day.

[Müřlıń®]

quote:

---

yes i too find some streaking lines on my copper electrode after using filtering

---

Is this in 2-d or 3-d?

Which toolpath gouged?

 

 

quote:

---

Has anybody else expiremented with these setting for best results?

---

I set my total tolerance at .001 with 2:1 filter and turn on arcs on all 3 axis. It works ok for me but I am not using micro mills and taking .001 stepovers....

 

The smallest endmill I use is .125 most of the time with .005-.007 step.

 

Murlin

[JG]

I to have noticed "streaking" due to arcs seemingly created "randomly", also I have used "other softwares" that filter to arcs and have not had the same issue. I actually ran the same part under the same surface-toolpath-filter settings and the "other software" made a much smoother part, sorry for the negative info, but its the truth. I think the "other software" looks at the whole surface first, then aligns the arcs as best it can before output.

 

just a guess

[Müřlıń®]

I know that the "filter" setting in Mastercam will try to smooth out the toolpath due to uneven geometry. The arc filters just use circular blocks on the arcs.

 

If you choose a loose tolerance on your filter settings to make your cuts smoother on crappy geometry, then you will probably have to turn off the arc filters. I would not use arc filters on anything greater than .0005 overall tolerance if you are to need a perfect finish like electrodes or molds.

 

Most of us use very good geometry made from solids and so one wouldn't need to try to smooth out the cutterpath. Loose filter settings are for cutting rough STL files. You can get a smooth finish out of a rough model using the filter.

 

So choosing a tight overall tolerance(.0005), will force the filter to follow the actual surface more closely. When doing so your arc filters will be much better.

 

Having said all that I would like to know the actual filter settings used to compare with the "other" software and the type of geometry being machined.

 

Murlin

[wildcat99]

quote:

---

Has anybody else expiremented with these setting for best results?

---

The last aluminum part I cut with a ballnose using Finish Scallop, .020 stepover, .001 Cut Tolerance and No Filter. There was definite "servo-studder" leaving dwell marks in the part.

 

Our next aluminum part will be cut in a week or so. I've programmed Finish Scallop and Flowline cuts with .020 stepover. Here I will try .00005 Cut Tolerance and .00045 Filter Tolerance with Arcs turned on at .005 min and 100.0 max for the final cut. I also have .0003 Cut Tolerance and .0007 Filter Tolerance with arcs set for some of the "roughing" paths before the final cut.

 

I will post here with the results of this "experiment" when done.

[crazy^millman]

Well I can tell you the changes I have had with finding my favroite thing which is filter. Cleaner looking surface and better looking parts all the way around and not the studders I use to get the other pre/arcfilter find. I am running a 2200 surface part right now that has 3 1/2" flat areas on it the whole part the rest is all curved surfaces ad nthe part is about 10" diameter and has to be optical clear acrlicy when it is all said and done.

 

Crazy Millman

[Rekd™]

quote:

---

10" diameter and has to be optical clear acrlicy when it is all said and done.

---

/me expects to see some picts..

 

'Rekd

[wildcat99]

I finished cutting our latest aluminum parts WITH filter. No servo-studder marks and the cutting time was quicker. I couldn't really tell any difference in the 2 filter settings, but this is not an aerospace part and I used a relatively large (.020) stepover for the finish cut.

 

There was some hesitation in places leaving transition lines where the cutter changed direction, though. For example, on a finish scallop cut there was an "x" left in the surface. The 2 lines of the "x" being where the cutter changed direction. I think the highfeed machining option would help here, but I've never used that.

 

Thanks for your suggestions, I hope this info can help someone else.

 

Millman, where are those pics?

[Fig sign]

quote:

---

There was some hesitation in places leaving transition lines where the cutter changed direction, though. For example, on a finish scallop cut there was an "x" left in the surface. The 2 lines of the "x" being where the cutter changed direction. I think the highfeed machining option would help here, but I've never used that.

 

---

In filter settings use one way filtering !

 

Do you use it ?

 

Now listening Sweet "Funny Funny "

 

[ 10-28-2003, 04:50 PM: Message edited by: plasttav ]

[crazy^millman]

Well guys its a freaking prototype and the customer will not allow me to post them up. I wanted to put it on the website but they felt like someone might try to take from their idea before it got to market. I am working on an update to the web site going to put up some video as well as some cool pics.

 

Crazy Millman

 

[ 10-29-2003, 12:58 AM: Message edited by: Millman^Crazy ]

[Müřlıń®]

quote:

---

though. For example, on a finish scallop cut there was an "x" left in the surface. The 2 lines of the "x" being where the cutter changed direction.

---

This happens when your machine tool has a little slop in it or you were taking off too much material with your finish pass and your cutter is pulling and pushing.

 

You should see what Scallop does on my 25 year old mill....heh it leaves about a .002 step where the direction change is.

 

But on my new machine, the same toolpath, the transition is seamless.

 

 

Murlin

[wildcat99]

Our machine is a 5-ax router, not built for heavy duty machining. Is .020 deep with .020 stepover and a 1/2 ballnose too much material for the finish pass?

 

One way filtering? This must be a ver 9 thing, because I don't remember seeing it in 8.

[crazy^millman]

Hey Wildcast since I think it might be like a Thremwood yeah you are going to get that on that machine you need to check your backlash on Axis B and Axis C I found it jumped it alot when machining Alum. Did your com[any but the heavy Duty machine or one of the Ligher Quintex Machines. They are looking at a Thermwood or some other 5 axis router and I keep telling them not to expect ot cut aluminum very well and salesmen keep saying we sell these for Areospace work and I keep trying to explain that they are good for Ren-Shape some plastics and thing of that nature and kick but they also hold pretty good tolerance on those materials but anything else I dont see them being that rigid. What do you think wildcat?

 

Crazy Millman

 

[ 10-29-2003, 01:08 AM: Message edited by: Millman^Crazy ]

[wildcat99]

I guess you would call our machine medium duty. We cut a lot of foam patterns, fiberglass and other plastics. It's worked fine for what aluminum we've cut so far. To keep chatter down, especially on the rough cuts, I take small steps, use stubby tools where I can and keep one hand on the feed override to slow down when needed. It seems to me you can use speed to your advantage with a router to make up for rigidity, large depth of cut, etc.

 

Our surface finish has been acceptable for what we are doing. At this point I wouldn't recommend cutting tight tolerance, exotic material aerospace parts on our router, though. But I'm still fairly new to all of this and as far as I know anything is possible!

[crazy^millman]

Well I cut Molds out of Aluminum on our routher and it was a wood router s oyeash it can be done but I found about .002 chip load was the most it would handle for finishing but since I had 18,000 rpm that was a good feed rate in most cases, I did the same .02 step down very high polished no honed edges very sharp postive tools. I found soemthing esle that worked good router bits that look like burr the kick but on fiberglass and composties as well xxxx aluminum but you got to mist the crap out of it. If I were you would put an aluminum plate up and damn around it with pucky or soemthing like that and then put your aluminum parts on that and ru nthe mister to keep your wodden boxes from gettign wet if you are using them. I dont recommned super high helix endmill round they chatter more than anything. I also used LH cut endmill put down forace on my materails that helped with chatter also.

 

Crazy Millman

 

[ 10-29-2003, 10:29 AM: Message edited by: Millman^Crazy ]