Smoothing toolpaths

[Brian B 74]

For those of you who create HST for machines with high speed controls - do you smooth your toolpaths in the filter settings? Or do you let the control do the smoothing for you? I had a job for our Roders that i set my tolerance to .002 (no arcs - best surface quality giving me cut tolerance of .0002" and smoothing tolerance of .0018"). It gave me a not so nice surface finish (using 1/2 2fl carbide ball).

 

We dropped the P/L .005" and I reposted the tool path witha .0002 tolerance (no arcs - no smoothing). Finish came out much better.

 

Looking for some thoughts on this.

 

Thanks!

[peon]

Brian, I program all of our molds with a .0002" total tol, smoothing settings to best (.00001" cut tolerance). I think your total tolerance is not near tight enough. I will use .002" total tolerance when roughing stock within .002"-.003" I have experimented using a .001"-.002" total tolerance for finishing in the past and had very poor results now and then.

[Brian B 74]

I have used those tolerance before and it made my mcx files HUGE and took FOREVER to verfiy the toolpaths. Thinking about trying .0002" total tolerance (.0001 cut tolerance and .0001 arc filter) to get smaller toolpaths. My post will automatically convert arcs to lines. I just don't have the time to sit there while verify backplots the toolpaths.

[peon]

Yep Brian, that is the tradeoff. Waiting for the damn verify, but we also saved some loot by reducing the workload on the polisher. I dumped the Quadro Card (fx3500 and fx1800) and installed a GeForce GTX 460 about a year ago. Made a huge difference in the verify speed but not the same as changing the tolerance. Adding arcs to the filter will also dramatically improve the verify speed as you are suggesting.

[Roger Peterson]

The Roeders does not like arcs, in fact the more consistantly spaced code the better for finishing toolpaths. Try a .0002" total tolerance set to 50/50 utilizing the fixed segment length (which is actually a max distance length). Then you have RMAX, RADMAX, etc... to smooth out the program at the machine.

[pip]

go with Roger on this one. We dont filter the toolpath at all with mastercam, we let the roeders do all the smoothing work. The dynamic settings on the roeders with 4.2 software is the best.

[Brian B 74]

I am filtering in the arcs just to make the toolpath smaller and the verify faster. The post converts all the arcs to lines (to a .0001" tolerance). No complaints yet.

[pip]

Brian

How large are your programs?

On average our nc files are about 20mb, with a couple going upto 200mb. Mastercam verify is soooooo slow with these large files.

[Brian B 74]

With my tolerance at .0002" (.0001 cut and .0001 arc tolerances) the file sizes aren't too bad - around 20-30mb. If I do the .0002" with smoothing all the way up the file sizes get into the 150-200mb sizes. AND they become tough to work with. Verify is extremely slow and I cannot live without that.

[Millertime]

Brian

When smoothing youre toolpaths do you use fixed segment length or shift points or leave those settings unchecked.I am kinda new to refining the paths.So far im getting pretty good surface finishes on my cores and cavitys. but I think that it could be better.

[Brian B 74]

Millertime - When I smooth I leave those unchecked. Right now I am experimenting without smoothing (letting the control do the smoothing for me).

 

Roger - What do you set your RMAX and RADMAX to? Curious if our settings are in line with yours.(RMAX = 4 for ruff, 1 for fin and RADMAX = 3000). Do you use TOL and SM as well? We use .0006 for fin and .0015 for rough on both.

[Brian B 74]

Revisiting this post. Have been told that size is becoming an issue. Round electrodes are coming out oval. Reading in the Roeders book I think I can tighten up my TOL and SM dynamic settings. Anyone want to share what their TOL and SM settings are set to for finishing?

 

Thanks in advance!

[crazy^millman]

I would recommend going back to the advice given. Tighten up the tolerances and see what your results are. On Round features I would always want G2 and G3, but if you tell it not to then will have to make the program huge to make sure you do not run into the very issue you now seemed to have found.

[mig]

Yep Brian, that is the tradeoff. Waiting for the damn verify, but we also saved some loot by reducing the workload on the polisher. I dumped the Quadro Card (fx3500 and fx1800) and installed a GeForce GTX 460 about a year ago. Made a huge difference in the verify speed but not the same as changing the tolerance. Adding arcs to the filter will also dramatically improve the verify speed as you are suggesting.

Is gaming card works better?

[Brian B 74]

No GeForce here. Boss upgraded my computer and it came with an AMD FirePro 7900. No real issues with MCX.

 

I have all the tolerances in MCX tightened up to under .0002". I am thinking about dropping the TOL and SM in the machine dynamics down to .0002 and see what happens.

 

Thanks for the help!

[peon]

Mig, with X5 and X6, the gaming card worked better than the Quadro FX1800 and FX3500 on my workstations. With X7's new verify, the Quadro 2000 is MUCH faster than the two gaming cards I mentioned on my workstations.

[Roger Peterson]

On a machine like the Roeders with advanced lookahead functionality, and depending on application, a good starting point for the fixed segment length (actually a max segment length) is 5% to 10% of the cutter diameter assuming you are finishing with a ball endmill.  it's easy to make a change and compare to your existing toolpath in backplot, just turn on the display endpoints function.  You may have to go even lower than 5% depending on application 

 

 

Having the post linearize arcs based on chordal deviation is no the same as outputing code at a fixed segment length.  Using chordal deviation will create relatively long moves based on the arc radius.  Fixed segment length will give consistantly spaced code even areas of relatively low curvature.

 

HTH

[Brian B 74]

Thanks for the response Roger.  My boss and I were at an AMBA supplier meet and greet and CamTool was showcasing their software and had some sample parts.  My boss was looking at the parts and looked at me and asked why the parts we machine didn't look like that (they were almost a mirror finish).

 

So the past 2 days I have been doing research on my arc filter settings and I started looking at my smoothing settings.  I think that is where I am going to start.

 

We finish all our mold cores and cavities in our Roeders so I know the machine likes the point to point code.  I am going to try a fixed segment length of 5% on my next job (ball cutter finishing).

 

I appreciate the help with this,

 

Brian Bylls

PM Mold

[Redfire427]

Brian,

 

I would be very interested to see what kind of results you get, or what you find works best. Our Makino's like lots of code too, but finding the perfect setting is a bit of a guessing game.

 

Carmen

[mike93]

I wish I knew what was best, but i do know some cad files with simular shapes, and same tolerence (.0002) 60/30 no smoothing same step over will go from fasets, to polished smooth???

[The Chipmaker]

 

My boss was looking at the parts and looked at me and asked why the parts we machine didn't look like that (they were almost a mirror finish).

 

 Brian that is a smoke and mirror deal. Parden the pun. Of course they have a mirror finish. A) How long did it take to cut? The geometry was probably perfect for a toolpath. Big arcs sweeping transitions. You would loose your shirt running the speeds and feeds and stepovers. There is a tipping point machine time vs. polishing time. 

[Brian B 74]

I know.  My boss was more or less looking to see if we can improve on the surface finishes to help reduce the polishing costs.  I have some programs in the shop right now with some new filter settings.  Waiting to see how they turn out.