Filters and tolerance

[Web]

Please share your experience in the use of filters and tolerance in surface finishing operations  To get a perfect surface

 

[BenK]

This topic has been brought up a few times over the years. Have you tried doing a search? One thing I will say is the settings can be very machine specific. 

[THEE THAINZ™]

Also results can very depending upon your choice/type of cutting tools used.

[Web]

This topic has been brought up a few times over the years. Have you tried doing a search? One thing I will say is the settings can be very machine specific. 

Yes, I tried to search, but could not find the exact answer, all the recommendations of the different

[Reko]

Yes, I tried to search, but could not find the exact answer, all the recommendations of the different

 

There are many recommendations because of many factors such as machine limitations... like anything else, the more options you have to really dial something in to your needs... the more complicated it can get... here is a good starting point:

 

 

 

30% cut tolerance

70% Line arc tolerance

I am assuming your machine can cut arcs in all three planes, hence the check boxes

no smoothing

 

If you can, post the details of the machine you are using ( maker, controller, options, etc. ), then post up some pictures of the surface finish you are getting with these settings... then you will get a lot of help with suggestions for your machine tool to get better finishes and results!!!

 

Good Luck!

[Web]

There are many recommendations because of many factors such as machine limitations... like anything else, the more options you have to really dial something in to your needs... the more complicated it can get... here is a good starting point:

If you can, post the details of the machine you are using ( maker, controller, options, etc. ), then post up some pictures of the surface finish you are getting with these settings... then you will get a lot of help with suggestions for your machine tool to get better finishes and results!!!

 

Good Luck!

Thank you! I use Fanuc  0md . When need use smoothing?

[Reko]

Using smoothing produces a lot more code... small segments that you can randomize, minimize and eliminate arcs altogether, if you so choose.

 

If you use this, your controller definitely needs high speed machining because of the large amounts of code generated. If used with the proper setting for your machine, you can get excellent finishes that require very little polishing... but again... it depends on what you are trying to achieve with the equipment you are using.

 

If you want to experiment with smoothing... I think your controller would use a G05 ... but I have not used a Fanuc in a long time, so perhaps others could chime in to give a bit more advice.

 

The main thing for you to do, is try the settings I gave you, then post your results... watch the machine run... give us some feedback... post some pictures of your results.

 

Then, you can test other settings and compare your results to your first attempt.

 

As others have stated... it is really a process... based on your time requirements, surface finish requirements, machine tool, controller, end mills, etc.

[Matthew Hajicek - Singularity]

 

30% cut tolerance

70% Line arc tolerance

I am assuming your machine can cut arcs in all three planes, hence the check boxes

no smoothing

 

I do the same but 20% / 80%.  .0004" tolerance for surface finishing.

[cherokeechief79]

try using create arcs in other workplanes besides xy.

loosten up the tolerance a bit and be amazed!

[Mjölnir]

I do the same but 20% / 80%.  .0004" tolerance for surface finishing.

 

similar here.

 

35% / 65% & .0002" tolerance for most finishing. arc fitting or not is machine dependent.

[Web]

Thank you!

I just tried to use the filters in the Dynamic Milling for roughing operations 

I use total tolerance 50% stock to leave

Cut tolerance 20% line/arc tolerance 80% and arcs in G17 XY and on machine aicc - G05.1 Q1

 I asked this question because I have very small experience in surface toolpaths

[Micromoldmaker]

It takes some experimentation to achieve the finishes you want.  I have a new computer now so I don't hesitate to go to .0002 or less on tolerance on final fishing as the processing time is not an issue any more.   Like other people have said: you have to work with the limitations of your machines and control.  If you have a computer that can crunch your tool path fairly quick you can tighten the tolerances to your liking.  It takes time to master all the surface tool paths, so keep at it and good luck.  Any questions in particular and you will always find someone who can provide you an answer here.

[Bob W.]

You really need to determine what the machine likes.  The bottom line is the machine needs to run the code smoothly and you will get good results so you need to experiment a little by posting code and running it.  My best luck has been to eliminate arcs and run strictly linear code.  I turn off arc filtering, turn on smoothing, use a fixed segment length of between .020 and .004 depending on the size and characteristics of the surface, and present arcs as line segments.  On the Makinos this will yield a surface that is perfect with no post machining finishing (.005-.0035 stepover).

[Gary]

You really need to determine what the machine likes.  The bottom line is the machine needs to run the code smoothly and you will get good results so you need to experiment a little by posting code and running it.  My best luck has been to eliminate arcs and run strictly linear code.  I turn off arc filtering, turn on smoothing, use a fixed segment length of between .020 and .004 depending on the size and characteristics of the surface, and present arcs as line segments.  On the Makinos this will yield a surface that is perfect with no post machining finishing (.005-.0035 stepover).

Yes shop down road with makinos and they like this, If I use smoothing on are new vm3 haas it looks nice but I can only achieve about 50ipm actual speed even if I program 400. Its smooth and not jerky just slow.