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?

Similar Threads:

• Guitar neck machining strategies
• Just IN- CAD-CAM Software - Dynamic Machining Strategies for 2 Axis CNC Machining
• Introduction to 3D Machining Strategies
• Part creation strategies?
• Chip thinning strategies, trochoidal toolpaths, high-speed machining using Mach 3?

[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]

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

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]

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.

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]

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.

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.

[Brakeman Bob]

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..

The biggest gripe I have with HSM roughing is the lack of control when the tool engages the stock - I like the "normal" or "tangent" approach / links in the standard 3D. I also like the "work only on rest material" option in standard 3D where the machined stock is generated by SolidVerify; if you have blocked out the part in 2D geometries (perhaps because you need flats to drill from 'cos you drill isn't long enough to go to depth from raw billet) HSM just doesn't recognise the previously machined stock. I think this is a hangover from HSM's mould & die roots and I see the logic behind it but for what I do, well it makes life hard for the programmer (me).

[JerryFlyGuy]

ahh.. ok well it sounds like your driving it harder than I . Most of what I'd done w/ it has just been simple molds and relatively un-complex 3d parts where I don't have alot of operations w/ very specific control over the operations. In those cases I can just 'point and shoot' and the results 99% of the time are just what I want.. the other 1% I've got to mess w/ it a bit.. to get some little nuance of the toolpath the way I want it.

Thanks Bob..

[Brakeman Bob]

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..?

No sir, I make brakes for racing cars. Everything from F1 down (though not a lot in F1 lately 'cos they haven't got the downforce to make use of big braking power without locking the wheels up). We do some stuff for WRC and I know that vehicles fitted with our gear have competed in the Baja 2000. Done a bit in NASCAR lately. It is interesting work. I was associated with the aircraft industry for 20 years and I love the pace at which things happen in motorsport.

[mattpatt]

Bob, would love to see some of your products.

20 years ago I was a young boy, working as a programmer/operator in a factory in the UK making very boring parts for cigarette manufacturing machines. I worked the night shift, so I used to sneak in some parts at 'lunchtime' for my race bike :-)

I never dreamed that 20 years down the road I'd have my own CNC VMC!

Now, I'm designing, programming and manufacturing parts for bikes, which we export worldwide, and also some one off stuff for the local car racers. We've got a few boring jobs for.......don't know what they are! They're not at all exciting, but bring in the money so must not complain.

Solidcam has been a great help with getting the stuff done quickly and efficiently, and I can't see myself changing to another CAM system just yet, even though I don't always get 'exactly' what I want from the generated toolpath.

[Brakeman Bob]

Gentlemen, I'm flattered.

OK, we have been subject to a "customer success story by SolidCAM" - http://www.solidcam.com/portal/pics/...N_EN_ebook.pdf

The calipers in the story are 'old school' - the stuff I am programming these days looks very different. Without a five axis machine the new stuff would be so difficult to machine (I have had over 30 MAC positions in one program) the would be well nigh impossible. We are mentioned in Raybestos' latest press release (Martinsville) but no pictures I'm afraid.

[MechanoMan]

Now I tried a part that would be cut out of bar stock with HSM.
So I tried "Auto-created outer silhouette", set Tool to External and gave it a bit of offset to rough out the part. That seemed to work OK though I actually need to work on specific surfaces, since we can't cut the whole thing out, there have to be some tabs or it'll fall free of the clamped stock during the roughing stage which would be destructive to both the work and the bit.

I try to switch to selected faces, set Tool to External, but I get "Cannot prepare geometry files!" when I Calculate.
Well, I haven't change anything under Geometry since the first run.

I went into the "Boundary File" and found it had created a crazy number of chains. I deselected all but the "big" one that appeared to encompass everything anyways. Looked at Show for Tool on Working Path, it looks valid for what I wanted. Still get "Cannot prepare geometry files!"

Any suggestions?

EDIT: Hmm, I was able to get a result by going with Manual "Silhouette boundaries" and selecting a set of faces I'd previously created for it. That does get around the "Cannot prepare geometry files!" but it's kind of a roundabout way of doing it.

Actually what I'm seeing now is the 3D Constant Step-Over, External Tool On Working Area with a small offset to allow it to back off the work has a problem. Where the toolpath starts/ends a pass near the end, it does this big wide curly-q to lead-in and lead-out (colored green in Host CAD Sim), I guess that's to reduce the acceleration on the machine, but it's venturing into un-roughed parts of the stock which will likely overload the small bit and snap it off. This exceeds the Constraint Boundaries, and it's well beneath the Upper Level so it's not legal to be there. The Constraint Boundaries are just the Drive Boundaries with a trivial amount more Offset. I guess I could rough out much more to protect it but this takes time, bit wear, and just seems like the wrong way to solve it.

And tests show that this is Lead-In/Lead-Out radius. If I change those to 0 the curls go away. I suppose it'll work ok without using them, but why is exceeding the Constraint Boundary permitted during Lead-In/Lead-Out moves? Isn't there some way to do Lead-In/Out in a way which doesn't violate Constraint Boundary?

[mattpatt]

Although I can't answer your questions directly, I too have had similar issues while using selectd faces. Since I have been using HSM more and more recently I tend to sketch my own geometry and let the tool work inside that.

It's taken a while (and I'm still learning) but I can usually get what I want done with the minimum of fuss. And the biggest bonus I've found with the vertical lead in/out rads is the lack of witness marks on the machined faces. I found I could feed in faster using HSM compared to 3D machining.

[JerryFlyGuy]

Can you offer any pictures of your part? For tabbed parts your going to have to create a sketch for the boundry or 'path' and then use just a simple 2d roughing program to cut the profile while leaving the tabs.

Another option would be to use HSM to rough the majority of the part out but limit the depth that it roughs to so you have enough material still holding the part in. Then switch to a finish operation and profile out the last little bit.

Can you describe the various machining process's your wanting to do to complete the job. Ie; Face, rough ex, rough interior, Drill, finish interior, Chamfer, finish exterior.?

once we have alittle more info I'm sure we can find your solution

J