PDA

View Full Version : Please Critic My Machining Strategies for this part



Schitzo
03-26-2009, 12:28 PM
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
http://img115.imageshack.us/img115/8619/throttlebody.jpg

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
http://img142.imageshack.us/img142/4599/tbroughcut.png

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

Results
http://img145.imageshack.us/img145/9594/tbsemifinish.jpg

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
03-27-2009, 04:20 AM
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
03-27-2009, 10:19 AM
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
03-27-2009, 02:08 PM
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

http://img13.imageshack.us/img13/8606/tbfinish.png

JerryFlyGuy
03-27-2009, 04:00 PM
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
03-28-2009, 12:03 PM
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
03-28-2009, 12:23 PM
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. :cheers:

JerryFlyGuy
03-30-2009, 10:25 AM
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
03-30-2009, 05:49 PM
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
03-30-2009, 06:02 PM
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
03-30-2009, 08:13 PM
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
03-31-2009, 01:12 AM
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
03-31-2009, 02:28 PM
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
03-31-2009, 02:33 PM
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
03-31-2009, 02:47 PM
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
03-31-2009, 11:47 PM
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
04-01-2009, 03:04 AM
Gentlemen, I'm flattered.

OK, we have been subject to a "customer success story by SolidCAM" - http://www.solidcam.com/portal/pics/products/success_stories/pdf/SolidCAM_ALCON_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
08-26-2009, 03:19 AM
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
08-26-2009, 09:53 AM
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
08-26-2009, 02:19 PM
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

MechanoMan
08-26-2009, 05:51 PM
Yeah, I know the partial-depth machining. But it's a double-sided part, the first side is roughed and finished slightly more than 1/2way through then we manually remount it upside down. As such some surfaces must not be cut out before the very end since it will release the part.

Hmm, I've got a 2D sketch with a vertical line meeting a Spline Path, then it's got a slight Radius. This is straight extruded into a 3D solid, and the edge between them is given a slight Radius.

Under HSM, the Boundary is Manual, Select Faces. I selected the 3 surfaces. This results is TWO Boundary chains, the Spline curve and Radius is one and the vertical line's surface is another. This is bad, it's a contiguous surface so the toolpaths need to be contiguous.

I looked carefully and there's no thin surface between them I'm missing and no extra Points on the 2D Sketch. In fact I went back and Suppressed the Radius feature, Synchronized, but I STILL have 2 Boundary chains for the pair of surfaces in HSM.

MechanoMan
08-26-2009, 07:57 PM
http://img36.imageshack.us/img36/4664/solidcambound.jpg

Well like here's where a straight line meets with a large radius. It's a simple straight-walled Extrusion. That's the display of the Boundary chain. It makes them two separate surfaces, so the toolpaths won't join up. I thought there might be some very small sliver of a surface between them that I didn't select, but no, there is not.

I tried increasing the Tolerance factor when selecting boundary faces... but that doesn't do anything.

MechanoMan
08-27-2009, 12:58 AM
Yeah so 3 have these 3 surfaces selected:
http://img103.imageshack.us/img103/9715/trigboundary.jpg
Which has the dreaded separation into two boundaries as previously described, but it's quite small and the problems in finish wouldn't be gross.

This is what I get for Tool on Working Area=Extern, with a bit of positive offset:
http://img354.imageshack.us/img354/8872/trigworkingarea.jpg
Which shows the toolpath areas overlap, so even though there are 2 paths, together they should cover all of it. It wouldn't be working as intended, but it should get the job done.

But the actual Constant Z machining operation:
http://img368.imageshack.us/img368/8209/trigroughing.jpg
The way I interpret this is the overlapped area between the two paths in Tool on Working Area (purple) is actually excluded from being covered by EITHER path. This will NOT work.

And trying the same thing with Countour Roughing shows, yes, that's EXACTLY what problem SolidCAM is having:
http://img269.imageshack.us/img269/5245/trigrouging.jpg
Because it draws lines around the overlapped Tool on Working Area zones perfectly! Well perfectly wrong... Won't create the part correctly.

I'm also curious why it always groups the boundary for the radius with the curved spline above it, never with the straight line below it. And as previously noted, even if the radius were not there it'll still make the spline and straight parts two separate boundary loops.

Also curious, if I try selecting only the straight face and the radius, and NOT the spline, it still breaks that into two boundary loops. And recall that with the radius suppressed, it still would not group that straight face with the spline. Actually, if I select the surface on the other end of that line- which is a straight line 90 deg offset- I get a third toolpath. Now that doesn't surprise me that much, because some toolpath generation avoids going around 90 deg corners, IIRC due to the huge acceleration needed to maintain a fixed surface speed or something. In that case it just makes 2 nonoverlapping toolpaths. But the radius makes no sense to separate from the line, there's not even a discontinuity in the tangency of the two surfaces where they meet.

Brakeman Bob
08-27-2009, 03:01 AM
A method I use for tabbed parts is to create a new part in the SolidWorks assembly by simply clicking on the menu "insert" then "new component". This puts an empty part in the assembly (and it offends me to leave it un-named so I call it "Tags") which I then fill with surfaces referenced off the DesignModel depicting my desired tabs. Then for 3D and 5 axis work it is a matter of (a) creating a new geometry called "TAGGING" and putting both the DesignModel and the contents of "Tags" into it and (b) setting the surfaces in "Tags" as check surfaces with an offset so the tool leaves a tab (or tag even!) of the desired thickness (I find 0.3mm works well with Aluminium). For the 2D stuff, I find having the surfaces there to see as I am defining profile sketches in the CAM part very useful.

JerryFlyGuy
08-27-2009, 10:45 AM
Have you tried creating a sketch and extracting the edges of the surfaces you want to work on and creating your own boundry that way? I've always found the 'automatic' type boundrys to not be optimum and sometimes down right un-usable. If you created a sketch on the part showing the region you want to machine on this might have better results than selecting surfaces.

At worst HSM while working on these sides like this may not be the best option [at least for a one off part] if it's a production part [runs of hundreds or more] then it might be worth beating on to get it to work..

Keep us posted..

J

MechanoMan
08-28-2009, 05:52 AM
Have you tried creating a sketch and extracting the edges of the surfaces you want to work on and creating your own boundry that way? I've always found the 'automatic' type boundrys to not be optimum and sometimes down right un-usable. If you created a sketch on the part showing the region you want to machine on this might have better results than selecting surfaces.

I'm not quite sure what you mean. How would you do that?
I'm doing the Select Faces most times, and let it generate boundary loops out of it (which it didn't do correctly). Are you saying draw loops manually in SW and try to bring them into SolidCAM?

I'm seeing where the non-HSM 3DM ops aren't running into this bug, so maybe I'll use that. Except the non-HSM has a completely different bug, where it will calculate the boundary totally wrong for certain curved surfaces, which appears to be a failure to use the Tool On Working Area and Offset fields AT ALL when doing Working Area->Work on Selected Faces->Drive Faces. It's there but has no effect on processing no matter what goes into it. Thus it generates an inconsistent, junk path on concave (and sometimes even vertical) surfaces because the surface edge is exactly on the boundary, sometimes it steps off the edge and machines all or partway down and sometimes it doesn't, probably depending on how the faceting got calculated internally. Basically it's viewing the boundary as the very edge of the face, but a face which goes vertical (or undercuts) has a conflict as to whether it sees the face edge as inside the boundary and calculates Z-level as the bottom (desired), sees the boundary before the edge and stops before it goes vertical, or drops to some totally unpredictable Z-value. Failing to go down to the bottom means the wall won't get machined which was essential. The resulting toolpath is basically noise.

And that's apparently because the Tool on Working Area isn't being used. See this is sort of what you'd expect from 0 offset, but giving it any positive value should have put the boundary past the face edge and solved it. You can give it any offset you like and it has no effect. In fact I can change to Internal, and give it a negative value larger than the face's width, which should keep ANY toolpath from being generated. Still generates. The field is totally unused.

And I've tried every single option in the whole operation, anywhere, nothing will fix this problem.

So I'm kinda thinking HSM for the curves that the 3DM can't do right, and 3DM for the straights that HSM can't do. Wow, that's kinda messed up but it does seem to be the situation and the answer.

MechanoMan
08-29-2009, 05:17 AM
Huh... ok... check out this workaround I discovered:

So:
1. 3DM won't work consistently on selected FACES which go vertical, because the Offset option doesn't apply properly.
2. The 3DM "Working Area" option didn't work because it works by defining a boundary via Solidworks edges. But picture a cylinder on its side, stuck to a wall. I want to go around the cylinder, but there is no "edge" on the side of the cylinder wall anywhere. There is nothing to specify. This option will not do what needs to be done!
3. When using HSM, when you Select Faces, you get these broken loops which HSM will totally screw up on. However, it turns those faces into a Boundary Loop in the process which gets thrown onto the main, shared list of closed Loops.
4. THAT Loop, created in the HSM interface, can then be selected for a 3DM operation as the Working Area. Now that it's a Loop and not Selected Faces anymore, the 3DM's Offset option will finally work, and the 3DM works beautifully!

JerryFlyGuy
08-31-2009, 12:15 PM
Mecho sorry, was away for the weekend. Just to clarify, to put a sketch in like my pic there and use that as geometry just means you jump over to SW [at the top of the feature tree] and add a sketch.. as simple as that..

Also, I've not tested it but the software SHOULD use the profile edge on your cylinder example to create a work area boundry... not nesc a profile boundry you can machine off off, because it's not really an 'edge' that you can select.. but it still should work as a work area boundry.

Fwiw

J

MechanoMan
09-02-2009, 03:01 PM
Also, I've not tested it but the software SHOULD use the profile edge on your cylinder example to create a work area boundry... not nesc a profile boundry you can machine off off, because it's not really an 'edge' that you can select.. but it still should work as a work area boundry

But it's not possible. When selecting Contours, they have to be made of lines. You can't select a surface by this method. A cylinder on its side, calling 0 deg straight up, we'd want to select a line at 90 deg, the top face, and 270 deg as our Work Boundary. But that's not possible, there's no lines there to select because it's a continguous surface. The top face has a line of course.

JerryFlyGuy
09-02-2009, 06:28 PM
I think we're saying the same thing.. :)

I agree that using the edge of the cylinder would not be possible in selecting a profile however if in constraints boundry you select the "auto of part" [I'm paraphrasing as I'm not in front of SC to copy it directly]

Then it should put in a boundry around the whole part so it has a work zone only.. I'm pretty sure I've done this in the past on a similar part [infact I know I have] and it worked then..

Fwiw

J

MechanoMan
09-03-2009, 12:07 AM
I think we're saying the same thing.. :)

I agree that using the edge of the cylinder would not be possible in selecting a profile however if in constraints boundry you select the "auto of part" [I'm paraphrasing as I'm not in front of SC to copy it directly]

Then it should put in a boundry around the whole part so it has a work zone only.. I'm pretty sure I've done this in the past on a similar part [infact I know I have] and it worked then..

Fwiw

JThat it does. That'll work for HSM, if you indeed want to do the entire part. 3DM, I don't think I've seen how to do that, but it's beside the point because I don't want to select the whole silhouette.

JerryFlyGuy
09-03-2009, 12:37 PM
If your wanting to only work on one section of the model vs the whole thing then you'll have to add a sketch [re: the picture I marked up] and then select that as your boundry.

Also, you can make a cylinderical wall into a profile [to machine along]. Orientate the model as it is in on the mill and in the plan view [X/y Plane Perp to the Z axis] insert a sketch and select the face of the cylinder and press "convert entities" it will create a profile of the outside perimeter of the part. Then you can use that for your profile.

One thing about CAD/CAM is if there is one way to do it.. then there's usually many different ways to get to the same result.. :)

J

Brakeman Bob
09-04-2009, 02:54 AM
One thing about CAD/CAM is if there is one way to do it.. then there's usually many different ways to get to the same result.. :)

Amen to that.