What does filter ratio setting do?

[bmilford]

I have been pulling my hair out over some large toolpaths/ files and someone suggested filtering my toolpaths. I did it and the toolpaths got much smaller. We where told by our instructor not to use filtering as the post processor for Thermwood Routers had some problems with it.

Can I create a toolpath with filtering on, verify it, and then change it to unfiltered? Would there be any difference in how the verify looks or how the file is posted?

 

Brian

[Guest]

With filter on there "could" be difference between your verify and posted code. It ultimately ALL depends on how your post handles arcs because ultimately that is what filtering does. It looks for moves based on your tolerance settings and and radius settings that it can put together and create one arc move instead of multiple lines, making smoother shorter code.

[crazy^millman]

It will also give you the ability to decide if you want arc moves on certain axis moves or not. You may want them on X,Y move but not on X,Z or Y,Z moves and you can control that there as well. I have also seen them help a machine run smoother because they are putting in the arc moves where and when you need them if doing a lot of surfacing toolpaths.

 

HTH

[dgriffiths]

I have used the filtering option extensively in the past posting to thermwood routers. With the kind of tolerances we needed for surface machining +/-.010 filtering caused no problems and most times resulted in a better surface finish of our molds. Make sure to only check allow curves in xy plane. I have had crashes on thermwoods when the other two planes are selected. I also had my post output 5 decimal places when using filtering because we had some number rounding problems with G2 and G3 when posting. HTH.

[crazy^millman]

Weird Dg I have run 120 hour run times on molds on the Thermwood with full filtering and never have that problem. I have done full 5 axis moves and everything with .001 filtering and get perfect almost no need to touch mold using the Thermwood.

[dgriffiths]

I only had the problem using certain operations. I believe surface finish parallel is one that gave us issues. Also our post was fair at best. Had several other issues. The number rounding issue was odd because I could never get it to consistantly repeat. The surface quality on the molds was actually very good using filter and like you I ran some very long run times. It is very possible that I just missed something while programming, just never figured out what it was.

[jeff]

quote:

---

I have run 120 hour run times

---

Are you re-finishing Mt. Rushmore or something?

That's a heck-uv-a-long cycle time!!!

At least from what I have ever seen.

My longest was about 8 hours on a 3 axis VMC.

[crazy^millman]

Was a mold that was 50" x 110" x 8" difference top to bottom and had about 10,000 surfaces and If I remember correct was a .003 step over with a .25 endmill. I left for Brazil and I was there a day and it was still running the same program. I think it was like 320 mb been about 6 year ago. Was cutting MDF so not a big deal. I think was 18,000 rpms at 200 ipm. Normally when I was doing prototype molds had 20 to 30 hour run times.

[bmilford]

Thanks all,

 

I am trying filtering, 2:1 with .001 tolerance, it has taken the size of the cutting file from ~5Mb to ~.8Mb. Pretty good considering when I started the initial cutting file size was ~500Mb.

 

Verify now seems to work, will verify give me any warning of a crash? or will I find the crash on the machine?

 

This is the mold that I am working on, it is 112.5"x30.5"x8" and is one quarter of the total project.

 

I am trying to cut an inside corner sharp, is there an easy way to do it?

 

Brian

[crazy^millman]

Nope not unless you got a 4th axis or 5th axis. They need to tell you the max allowable radius or you need to talk to a EDM shop and plan on some major bucks. Pretty simple mold. If I had to have the sharp corners I would make it a 2 piece mold and extend the spiral probably .27 to .52 longer depending on how thick it was. I would then cut off the excess and then mate the bottom plate to it making the sharp corners. The other things is the transitions would be outside the part. If you have a sloppy machine you would be cut off that area giving you a much better looking mold high quality mold.

[bmilford]

Well I have the 4th and 5th axis, the mold(pattern) is MDF. The sharp corners that I need are the inside corners along the edges of the spiral as it is 1/4 of the finished part and I need it to match up perfectly.

 

Brian

[crazy^millman]

Ok then I would do a 5 axis Multi surface doing .002 step downs taking out the radius left over from the 3 axis kellering or surfacing. Pretty straight forward toolpath and using a sharp endmill with that small of a step down should yield you great results. If you need help with the toolpaths send me just the model and I would be glad to throw some 5 axis toolpath on a part of it to show what I am talking about;.

 

HTH

[bmilford]

Ron,

I'm thinking about using a v-groove cutter and a 3D contour toolpath following the curve of the edge of the spiral. I may have to do a different toolpath in two areas, but I haven't gotten that far yet. I think that in those areas we could use a 1/8" ball end mill and live with the radius left.

 

Thanks,

Brian

[Colin Gilchrist]

Brian,

 

Don't try 3D contour, use Surface - Finish - Project. 3D contour may work with the V-bit, but will not work with the ball endmill. 3D contour does not do tangent surface offsetting of the toolpath.

 

HTH,

[machtek]

"B" I just completed a mold very similar to this (spooky really) and I made the negative of the part to sharpen up the corners. I only have a 3 axis currently or I would have done as Crazy suggested. Keep in mind MDF will only hold a radius of about 1/16 anyway. You will prolly have to move to a more dense mtl to hold sharp. My customer spec'd sharp no radius. We cast the parts anyway and he loved it. Hope you have the same luck.

 

Dennis

[Thee Starry™]

Sort of related....When I try to filter, my options to "create arcs in XY, XZ and YZ", are always greyed out in the filter dialog box. I can not check any one of them ever. Why?

Also, is it typical that a Thermwood Post will only use radius on XY? I can not get IJK for any radius other than on the XY plane and only when doing 3 axis work. If I am posting to the 5 Axis machines, I never get I,J,K for any radius. Any clue. No matter my GEO, all radius are very small straight lines.

[3R!< W3NG3R]

Starry, you have to set it in your control def>arc

[Thee Starry™]

I believe I have that all set

Support arcs in XY, YZ and XZ are all checked. Arc center type is Delta start to center for all 3.

[cadcam]

bmilford did you ever make it on to the FTP I see you were trying and not haveing success for a while.

[Thee Starry™]

bump

[bmilford]

No I haven't been able to get past the logon, but I haven't tried lately.

 

I would use my logon for the forums to get on the ftp, correct?

 

Brian

[bmilford]

Dennis,

It is kinda spooky, looks like you are using the same computer as well. How was processing time for the file you where working on?

 

Brian

[machtek]

I started on a P4 @ 3.2 ghz, it took sometimes 30 seconds per mouse wheel click to zoom in or out and to dynamically spin, maybe 1.5 min to update with shading turned on. I gave up on the project until the Zeon came in. When I resumed, to dynamically spin, it makes fluid motions. Totally smooth. To process the tpath, maybe 5 seconds on the Zeon (parallel surface).

 

I love my new Zeon ('s)

 

( a double cheers on this level of computers and CNC software)

Doing normal stuff, the computer is finished with one task before I can think up the next. Makes my mouse button finger and my brain sore.

Dennis

[dgriffiths]

I was using mostly V9 when posting to the thermwoods but always got IJK values for 3ax arc moves. We could not however get it to output G72/G73 3d arcs from our post. Probably not much help but thought I would chime in anyways.