Printable View
Hey guys,
I made my first part with the Tormach today (PCNC1100) and I was quite happy. But the surface finish on the sides are not great.
Here is my settings:
Material : 6061
Tool: 1/4in / 2 Flute
Step #1: Roughing - I do 2D contour with ramp, I leave 0.004in for finishing pass
Spindle: 5100
Feed rate: 17 in/min
Step #2: Finishing Pass- 2D contour with ramp,
Spindle: 5100
Feed rate: 21 in/min
Just a lathe owner here, but upping the speed and slowing the feed works for me.
My first impression was that the ripples on the end of your part are caused by balance issues of the motor and spindle. I explained this in a very old thread https://www.cnczone.com/forums/torma...ml#post1140470Quote:
Originally Posted by mendez
There was a lot of disbelief/opposition at the time but some have since come around. I estimated the width of the end of your part to be around 1.25" and the ripples per inch to be around 46 on the lower half. As your finishing pass used a ramp I assume the cutter passed over the upper half twice. If I feed these values into the calculation it works out almost exactly with your speeds and feeds. The spindle is not balanced (at least not on the pre-M series 1100's) and the motor fan was imbalanced by design. Balancing is probably not something you'd want to attempt but you could try simply removing the motor fan completely (at your own risk). My motor never runs for any long periods so the motor never gets warm anyway. I think it was nitewatchman (could be wrong) who made a 3D Printed adapter for a standard computer type fan, but I was planning to just mount a fan on top of the existing fan housing with a plate - I never actually got around to it.
At some point the imbalanced fan was replaced by an improved design but I've no idea whether the results were better.
I would normally also expect a wavy pattern on top surfaces with the same repetition period for the same reason. I think I can see something like this on your parts but (presuming you used a superfly) this can be quite difficult to eliminate completely. I assume you finished the top surfaces before profiling the part as you don't have much support left. I would perhaps consider improving the workholding as a plate like the one you're using will bounce around and flex a fair amount - even before the profiling op. I'd also be a little concerned about it pulling out of the vise.
Hope this helps
Step
That setup is too flexible. You need a sub-plate. Drill the hole pattern, then mount the stock, using bolts, to the sub-plate, then cut the perimeter.
Yeah, that's obvious chatter from a lack of work holding.
Tab workhodling is not great.
I would recommend getting stock that is 3.5mm thicker than you need for the part. Then hold it at 1/8" in the bottom, and profile it out, without tabs. Cut to slightly below the bottom of the part, which is slightly above the vise (hence the 3.5mm thickness margin!)
When you're done, flip the thing over, hold the PART in the vise (possibly with soft jaws) and shave off the 3.5mm bottom part. The vise should now be holding a complete part.
You can only do this with parts held horizontally -- your setup would have to reduce to two at a time in this case.
However, because the vise holds the entire part (and the stock holds the entire part when profiling) this will be much more rigid.
Yes, for thin parts, this increases material cost a little bit, but if material cost is the majority of your cost, you're not in the right business, because the Chinese will out-do you there no matter what!
I would make a fixture, drill and tap it, then drill all the holes in your part, then bolt it to the fixture plate and do the contouring and engraving. A nice rigid fixture will do wonders for the finish. I always run a finish contour of 5 to 7 thousanths to clean up the contour.
Thanks guys for the feedback. I started designing a fixture/pallet system using Mitee-Bites. I can have one fixture to do the first process and use soft jaws or another fixture/pallet for the bottom side. What do you guys think?
Also, is it possible with the PCNC 1100 to get mirror finish parts in contours / sides?
Attachment 443000
That seems easier than my idea. Thanks!Quote:
Originally Posted by popspipes
If the parts are bolted to the fixture plate thru the holes, you can do the outer contour as well. Maybe you have to face the top?? The contour wont be mirror finish but it will be a nice finish.Quote:
Originally Posted by mendez
Also I would space the parts closer together so that the cutter doesnt leave a solid piece in between the parts, if you are contouring them it can get hung up and break a cutter when it is cut free of the main part, plus it will save on material.
This is a small fixture for one of my parts, and a finished part, the phone doesnt take really good pics, but I think you can get the idea.https://www.cnczone.com/forums/attac...d=443004&stc=1https://www.cnczone.com/forums/attac...d=443006&stc=1
Thanks. Yeah, I will try to bolt the parts then. The finish is really good. Are you using 3 flute with coolant?
Attachment 443016Quote:
Originally Posted by mendez
This is an image from another old thread showing my results after balancing. You will see cutter marks, that's unavoidable, but they alone will still give you a very nice finish.
By the way, most people on this forum don't appear to be regulars here so they might not be aware that popspipes used to post under the name "mike sr1". He's the guy with the cool eccentric ring solution in the thread I linked to earlier.
Step
That finish is with a 4 flute, HSS endmill, 3 flute is OK as well, I avoid 2 flute, they work well , I just think the 3 and 4 flute are more rigid, just personal preference and I believe the finish is a bit better.Quote:
Originally Posted by mendez
The fixture needs to be rigid, that and vibration will affect your finish.
I use oil for coolant, flood, just my personal preference and the finish is better.
I agree with Mike's approach on endmills. Often use 2 flute for roughing to keep from clogging up with chips, then finish with 4 flute for rigidity.
Terry
I am a firm believer of 3 flutes for aluminum. That's what they're for! I used to use 2-flute, but 3 flute just allows me to feed 50% faster.
I've never had luck with 4 flute; they always clog, although I imagine on a very thin/whisper finish pass it might work, perhaps? The tool change would be a killer for time, though!
Regarding the fixture: I love it! Make sure to pack the parts tight if you're going to make tons of them. I never make more than a dozen of the same part, so I'm less inclined to make fancy fixtures :-)
I agree that the part spacing should only be your end mill size plus some margin. And you might want to use a 3/16 instead of 1/4 if you want to really pack them in.
It does work pretty well for finishing, for me, that is usually just a few thou, 5 or less and the mills don't get packed up at that size, Since I am just a hobbyist, and most of my parts are one offs, the time for a tool change isn't very important. If you have many parts to do it would be a different story.
Terry
As others mentioned above. Reducing machine vibration, work holding, tool chatter, gibbs on one or more axis not adjusted, bad feeds and speeds, tool runout ……………..... the list that can effect your results can be long. Work with the machine and do some testing if possible on fixturing, cam setups, cutters, over a little time you develop a style and methods that work for you. Learning curve can be kind of steep but with experience you start getting better results most of the time.
I use cam templates to load model part shapes into. They have standard operations setup that I know get good results. Those preset cam operations use what I now call my "First responders" :)
This is a set of tools I tend to use all the time by habit I guess. Starting with Hamier probe, Super Fly cutter, 3/8 y/g alumax 3 flt mill and a 1/4" c2 chamfer mill drill. Add drills and taps as your design requires and your on your way.
When you get a good cad/cam work flow going and some "first responders" in the rack its not hard to make shiny stuff.
Attachment 443052
Nice clean surfaces inside and out and chamfers are smooth with little faceting. Scratches from thread ops :(
Then as Tstep mentioned in an old thread how you can become obsessed with order of operations or ways to avoid scratching the surfaces.
btw: I have same "first responders" in router tool rack. E probe, 4 insert surface cutter, 1/4 c2, coated 2 flt router bit and 1/4 c2 coated 2 flt chamfer mill drill.
And same custom 24r cam templates for quick loading of models to setup ops on. This also makes working on different types of machines more straight forward with less errors.
Thanks Step for the compliment! I made mine out of aluminum with the thought of making a steel set later............ that was 8 years ago ha! Goes to prove the saying "If it aint broke dont fix it"....Quote:
Originally Posted by TurboStep
An excerpt from one of your posts Turbo.
Balancing is probably not something you'd want to attempt but you could try simply removing the motor fan completely (at your own risk). My motor never runs for any long periods so the motor never gets warm anyway.
Back in the day we had a pump running without a fan, one instance I am thinking about ran that way for years, it was a 5 hp pump on the Clean In Place system in the dairy, all our motors when rewound used an epoxy dip on the windings, maybe that was the reason it lasted so long without the fan.