Best Finishing strategy for this part?

[JVizzi]

I could use some help in learning about finishing strategies.

In the attached file I have three different finishing toolpath strategies I am working on. So far the flowline toolpath seems the most simple and smooth, but I don't know if it is better than scallop or contour. This 45 degree "cone" is a common feature on several other parts I need to program as well

 

Thanks,

[Tinyfxds]

The Hybrid Tool path will give a nice finish with few lifts.  .005" on the z depth and .005" on the stepover  and it looks like this

 

 

:

[JayM]

Some more information would be helpful to answer your question.  What tool do you use for finishing? What surface finish do you need?

 

Flowline is good for this part, or contour.  Both will give you similar motion.  You could also use the High speed spiral toolpath that should work well for this part.  I don't see any need to use the scallop toolpath.  It is a very simple shape so good choices are pretty open.  If there is a specific issue that you are having with flowline describe it so that we can address that.

[crazy^millman]

Flowline spiral works great on this part. You had one way with no direction options if you want one way and a constant cut then use spiral. If you want one way and lead in and out then use direction on the 2nd tab to control the end and out movement. Surface Finish Contour is another option.

[JVizzi]

Thanks for the replies.

 

The Issue I am having with the Flowline is that it gives nice smooth toolpath, but its all tiny line segments. But one I turn up the tolerance larger than about .005 it starts adding a bunch of rapid retracts.

 

I don't understand why its creating line segments, the geometry is a true circle all the way down

 

The program can't be too long because its going into an ancient controller/machine    '82 matsuura with Fanuc 11

 

 

Is the Solid messed up maybe?

[cherokeechief79]

ive been thru this lots of times myself.

in my opinion all of those toolpaths you used are crap.

the absolute and easiest way to get a beautiful finish on a single taper like that is to use something you would never think to use.

try using threadmill.use a ball endmillinstead of a threadmill  and in the angle box put the angle of your taper in.

for the pitch just put in the stepover you want.

you will be very surprised at how nice this will come out!

it will do continuous toolpath without a single zipper line or shift mark and you can even run cutter comp on it to tweak the size to exactly what you want.

[JayM]

 

The Issue I am having with the Flowline is that it gives nice smooth toolpath, but its all tiny line segments. But one I turn up the tolerance larger than about .005 it starts adding a bunch of rapid retracts.

 

Turn on tolerancing to get G2/G3 arcs

[crazy^millman]

ive been thru this lots of times myself.

in my opinion all of those toolpaths you used are crap.

the absolute and easiest way to get a beautiful finish on a single taper like that is to use something you would never think to use.

try using threadmill.use a ball endmillinstead of a threadmill  and in the angle box put the angle of your taper in.

for the pitch just put in the stepover you want.

you will be very surprised at how nice this will come out!

it will do continuous toolpath without a single zipper line or shift mark and you can even run cutter comp on it to tweak the size to exactly what you want.

 

Do you mean tapermill?

[crazy^millman]

Turn on tolerancing to get G2/G3 arcs

 

Also might try use the tighten filter tolerance as well.

[cherokeechief79]

Do you mean tapermill?

nope     threadmill.

[JVizzi]

Ok, I have G17 18 19 on now. Made it alot better. But still about 40k lines of code. Here are my current settings.

 

total tol. =  .010

stepover, distance .005

50/50 cut tol. line/arc tol

min arc rad .5

max arc rad 100

 

the surface finish needs to be 32. and my spindle is max at 3500rpm

 

How to I attach a pic of my desktop screen?

[JayM]

Here is an example with one arc move per step down.   About 500 lines using Mill default

M00006033-1.shorter.MCX-7

[cherokeechief79]

I just guessed at the angle.

200 lines of code no retacts and no shift marks.all arcs no line segments..005 step down,

for some reason I cant post the file here.

[cherokeechief79]

hope this goes thru.

M00006033-1 thdmill.mcx-9

[JVizzi]

John,

 

That is perfect, thank you!

 

But I don't understand, I put in your exact settings into my program and it comes about 1652k and yours is only 39k

 

What am I missing?

[JayM]

Try replacing the post in my file with your machine definition.  It could be something in your post.  If my program still comes out shorter their must be something different in our toolpaths.  Upload your file again and I will take a look.

[JVizzi]

ugh, forums.....how do I delete my old attachment, its saying I don't have enough space to attach another one?

[JVizzi]

Got it, here you go

 

 

Yes, I re-loaded my mach def and it still came out short just like you sent it.

[JayM]

Change your cutting method from "Spiral" to "One Way".  

 

It is a balance of what is important.  "Spiral" will give a toolpath with zero retracts but essential runs point to point, "One Way" will filter to a very short program but steps down between passes.

[cherokeechief79]

Here is an example with one arc move per step down.   About 500 lines using Mill default

very nice. ive never gotten  it that good using a surface toolpath.

but it does still have a zipper line.

threadmill will eliminate that.

[JVizzi]

Ok, yeah I missed that I still had it on spiral. Just seems counterintuitive, it should be if you select spiral and the geometry is a round, non-spline arc, it should come out one smooth cut, with one z move per pass around, kinda like a lathe.

 

I don't understand why it has to break it into line segments

 

oh well

 

Thanks so much for the help!

[JayM]

very nice. ive never gotten  it that good using a surface toolpath.

but it does still have a zipper line.

threadmill will eliminate that.

 

Yes a very clean way of getting short code from the program.  I have been trying to get the surface toolpath to output the same way, it just doesn't want to see the surface as a series of helix's.  

 

Another option would be to use Surface Finish Contour with the Ramp option turned on.  A short ramp between passes will usually eliminate the "zipper" line, depending on setup.

[JVizzi]

Just for kicks, I tried the contour finish toolpath, with ramp, but it has a ton of rectracts. Thoughts?

 

Also, how can I rough this taper. The stock has a 10.0" thru hole in it already from the waterjet. Which toolpath can I use that will pocket all that out, but also realize there is a hole already in the stock?

M00006033-1.MCX-7

[JayM]

Finish Contour will jump on the first couple of passes, especially with a very small step over.  You can eliminate some of these by setting Advanced Settings > Only between surfaces.  Also change your ramp length to a much smaller value, between .1 and .01.

 

For rouging the part you might try a large tool that can overlap all of the material left, and just use the same toolpath for roughing as finishing, just leave stock on the roughing one.  If you can upgrade to X9 I would recommend using Optirough with a Stock Model.

M00006033-1-3.MCX-7

[jlw™]

I'm a little late to this and I see everything I've done listed. I'll add that at times with a "funnel" shape like this I'll use 2d contour with tapered walls so that the op can adjust with cutter comp if needed. Just a thought.

 

 

I love surface finish contour, if I could have cutter comp on that... Favorite. To get it to stay down adjust your gap settings. Also you need to get used to using check stock and containment for surf contour.

 

HTH