Please Critic My Machining Strategies for this part

[Schitzo]

Hello all
I'm very new to cnc machining and looking to make the part pictured below. I working in solidworks and solidcam. I have come up with a strategy to make the part and hope you can critic what I intend to do.

Material: Al 6061
Machine: Benchtop CNC converted mill (X2) running Mach
Part dimensions: 2.5" x 2.5" x 2.5" (approximately)

Part


Once I have the stock faced to the correct dimensions,
I start with a rough cut
3D milling, 1/2" endmill, contour cut, 2mm step down and 50% overlap , 0.5 surface offset

results


then semifinish
3d milling, 1/4" endmill, Linear, 0.2 surface offset, 0.1 scallop

Results


Finish
3D milling, 1/4 ballnose mill, linear, 0.01 scallop, 0.01 arc approx

results look very similar to the diagram above

I just can't get a good finish. Any advice, is welcome. How would you machine this part?

[Brakeman Bob]

Are you programming in inches or in mm? If you are programming in inches your arc tol is far too big - try setting it to .001. You will get an lot more code, but the finish will be better.

[JerryFlyGuy]

Also, you could do a constant Z for the first 30-40 deg around the curve and then finish it w/ a constant step over in the same direction. I'm not sure I'd use around the cylinder, but rather along the cylinder. I just checked and w/ a 1/4" ball nose and a 0.01 step over you should have a max scallop of 0.0001" so it should look pretty darn smooth. How accurate is your machine [step resolution or steps/in in mach]? Also as was noted jump up the tolerance on the part. I'd go to something in the 1/2 thou range myself. It will generate LOTS of code but in tight finishing pass's it often dones and is required.. it shouldn't slow the job down any as in your finish pass on a X3 your not going a mile a minute anyway..

Fwiw

[Schitzo]

Originally Posted by Brakeman Bob Are you programming in inches or in mm? If you are programming in inches your arc tol is far too big - try setting it to .001. You will get an lot more code, but the finish will be better.

Bob, thanks for the insight.I'm programming in mm. I believe that is the default in SC. A change in the arc tolerance definetly smoothed things abit. see the pic below

Originally Posted by JerryFlyGuy Also, you could do a constant Z for the first 30-40 deg around the curve and then finish it w/ a constant step over in the same direction. I'm not sure I'd use around the cylinder, but rather along the cylinder. I just checked and w/ a 1/4" ball nose and a 0.01 step over you should have a max scallop of 0.0001" so it should look pretty darn smooth. How accurate is your machine [step resolution or steps/in in mach]? Also as was noted jump up the tolerance on the part. I'd go to something in the 1/2 thou range myself. It will generate LOTS of code but in tight finishing pass's it often dones and is required.. it shouldn't slow the job down any as in your finish pass on a X3 your not going a mile a minute anyway..

Hi Jerry thanks for the info as well. Im not sure I quite understand the 30-40 deg in constant Z. care to offer more info?
It looks like I was using a large scallop value hence the less than desirable finish.

I am still putting together the machine and should be done here pretty soon.


One other question, how accurate timewise is the solidverify feature? I have to make 8 of these puppies and it looks like a smooth finish might take quite a while. These are throttle bodies going on an V8.

Once again thanks and more insight is welcome.

pic with the current settings

[JerryFlyGuy]

One of the things I try and avoid is linear machining with a really steep wall, I'd much prefer to use a Z level machining in those situations.

Are you using HSM? I'm not sure if it's an option in the straight 3D but in HSM there is a setting in the passes window where you can tell the program you only want to constant Z machine on a wall that is steeper than 40 [or whatever number you choose [from horizontal] up to 90 [or vertical]. This will then get you your best finish in the steep area's. Then you can change it over to a linear or constant step over and use the same angle limitations [maybe increase the angle from 40 to 43 to make sure the paths cross/overlap] and you should get the best of both worlds.

Super smooth finishes take alot of time, often it's just as easy to get them 99% of the way and then hand finish [if it's just cosmetic]. Btw, that'd be a good candidate for a 4 axis job..

[Brakeman Bob]

The time estimation in SolidVerify is not reliable. For example, it tells me that to gundrill a Ø3 hole 160mm deep takes over 1 hour when it takes about a minute and half. For 3D stuff on my work (Ally mainly) I would allow about 25% more than SolidVerify says for that job only.
Jerry is right about diving down steep faces in a linear strategy and HSM is definitely the way to go - we saw a 20% reduction in 3D cut time switching from conventional 3D to HSM.

[Schitzo]

Originally Posted by JerryFlyGuy Are you using HSM? ..

Hi Jerry, Im not using HSM, I did all the work under standard 3D milling. Correct me if Im wrong, but isnt HSM out of the realm of my homemade benchtop cnc mill. I have the impression that code generated in HSM requires a machine that can work with it. I'm I mistaken? I still have alot of reading to do.

I will look under HSM later today and report back with my findings.I also have to agree a 4th axis would be great. I am not strict with design. If it prooves too difficult to machine I can always revise the design.

Originally Posted by Brakeman Bob The time estimation in SolidVerify is not reliable. For example, it tells me that to gundrill a Ø3 hole 160mm deep takes over 1 hour when it takes about a minute and half.

Good to know Bob. I guess when its all said and done, I have to cut a few practice pieces before I get to cutting alluminum that way I know exactly what to expect.
The intake Im working on, I got from a fella your side of the pond. Jenvey is the name of the place.

Thanks for help guys.. I appreciate it.

[JerryFlyGuy]

HSM is for any machine tool. I will take an old tired machine and bring it alive. In SC when your running HSM the tool can be set to arc in and out of every move so your not slamming to a full stop in one direction and then taking off in another. I don't see how using HSM would hurt you even on a small bench mill.

Fwiw

[Brakeman Bob]

Originally Posted by Schitzo The intake Im working on, I got from a fella your side of the pond. Jenvey is the name of the place.

I have just checked out their website, they're only 25 miles from where I live. It is a small world. Are you, like me, in motorsport?

I would second what Jerry says about HSM. We don't regret buying it at all - shorter cycle times, nicer finishes, impressive strategies, easy ways of setting work area, very kind to the machine - yes, it is really good. It ain't all honey & roses though - I still use conventional 3D for roughing because of the rest machining.

All the best

Bob

[JerryFlyGuy]

Bob, I'm curious as to why you don't like the HSM rest machining, or rather prefer the standard 3D rest/rough? Do you prefer the 3d over both the Rest rough and rest finish or just rough? I've not had too many occasions to use it but... it's worked when I did..

Fwiw

[Schitzo]

Thanks alot guys. I spent some time playing around HSM, still have some learning to do. I'll post up what I come up with.

Originally Posted by Brakeman Bob It is a small world.Are you, like me, in motorsport

It is indeed a small world. I am very much into Motorsports. I do some rally and autocross but nothing big. I mostly like building cars and its the reason I have gotten into machining. There are just to many times you have to fab up a part or two.
Do you race, build cars..?

[mattpatt]

I'm no expert, but I use HSM quite a bit now, but I do still struggle from time to time and revert to the 'normal' 3D strategies. HSM has more strategies than I know how to use!

As I design 99% of the parts that get cut on the machine I am slowly changing some of the older 2D designs to 3D, to take advantage of the capabilities of the machine. It really toots my horn when I see the finished part come off the machine.

You mention finishes and tolerances. It's funny because on one of the jobs I did my business partner moaned because I'd taken the time to put a nice finish and he claimed that it didn't look CNC machined! So now I have to hold back and try to show the cutting path on 'not so important' faces.

concerning tolerances, I usually stick at around 0.01mm for finishing, but sometimes go down to 0.005mm as this seems to get me a better, smoother tool path, with less Z rapid jumps. Takes longer to calculate, and gives more code, but the machine copes so why not.

But as I said, I'm no expert, however, as every job goes by I learn a new trick, which either reduces cutting time, or gives the finish I desire.