CNC part design consideration.

[RollingCamel]

Last year the upright designer didn't take machining design rules into consideration, neither did I have enough knowledge about it.

I have found a couple of resources:

http ://www . omwcorp . com/partdesign. html#2
http : //www .efunda. com/processes/machining/ mill_design. cfm

Some basic fixture design books will be helpful too. For your designs what do you use as a rule of the thumb?

[RollingCamel]

Last year the upright designer didn't take machining design rules into consideration, neither did I have enough knowledge about it.

I have found a couple of resources:

http ://www . omwcorp . com/partdesign. html#2
http : //www .efunda. com/processes/machining/ mill_design. cfm

Some basic fixture design books will be helpful too. For your designs what do you use as a rule of the thumb?

[Goost]

Hopefully on a part as complicated as an upright you have access to a CNC mill or can possibly have a sponsor machine the part for you. I do a lot of machining for our team, we fortunately have our own HAAS TM-1 vertical mill in addition to the manual knee-mills and engine lathes. Speaking from my little bit of experience, the biggest bother (and chance for error) is in part repositioning. We usually square, drill, and tap the stock manually one of the manual mills before any CNC machining is run (so that offsets can be made accurately and the piece can be bolted to a jig-plate). Here are a couple things I hope are thought about in our design phase, though often they are not:

1) It helps considerably if our part designers keep in mind that a three axis machine can only hold a tool vertically, so requiring cutting from more that one direction requires part repositioning.
every part repositioning = less consistency.
2) Also, if a part cannot be fixtured properly so that it is held stationary when broken free from the stock, there's a good chance you have nasty gouges in your final piece, not to mention broken endmills (A rookie mistake I admit I still make occasionally. I was once told you're not a Real machinist until you crash a machine; just something to think about...). Sometimes this requires moving the fixtures after half a part is made to continue on the other end. It's just a pain to do, and again there is a chance for some slight movement when the setup clamps are repositioned.
3) I think I'm just lucky, but Solid Edge default seems be 1/8" radii on corner rounds, so I can usually get away with using a 1/4" ball mill on most anything. Of course if the part needs a larger radius somewhere for structural reasons this is no excuse not to make it as the model requires. Sometimes on larger radii a 1/4" ball on a surfacing operation serves my need. Less tool changes/offsets = more consistency.

Of course there's a ton more information and far better machinists than myself out there but those are the ones that help me out the most. Also, the sources you listed definitely have very useful information.

Hope I could help!

[MegaDeath]

I think the biggest thing that will help anybody who is designing parts or the person who will be CNC'ing them is just good old experience with a manual mill. I never read any literature to learn the "how to" or "how not to" aspects of machining, probably 90% of my machining skills came from the older guys on the team and the other 10% I have acquired over the past three years. When I first got involved in FSAE I couldn't even turn on a bandsaw, fast forward to today and I have a job at a machine shop where I work as a CNC programmer and operator as well as manual machinist when it is applicable. And because I have access to top of the line machines and tools I do a fair portion of the CNC work for the team.

I personally don't believe that machining practices is something that you can accurately learn from a book or online article. In my opinion the BEST way to learn good CNC operation as well as manual machining skills is to simply learn from somebody else and gain experience and knowledge from them. To me there is no substitute for first hand learning and first hand experience.

[Jersey Tom]

I'd agree that there is really no substitute for experience... even if it's on manual machines.

That said, a few quick considerations before I take off for a disgustingly early flight-

1. Make use of common workholding, primarily the vice. That means putting parallel edges that you can clamp onto. The more rigid the workholding, the faster you can machine and to tighter tolerance. Also, minimize how many setups you'll need. Always think "How is this going to be held onto to machine this feature?"

2. Make use of large tooling where possible. For pockets, this means large inner radii. I am also a fan of using non-standard inner radii, a little bigger than the tool I'm thinking of using. If I envision a pocket being milled out by a 1/2" endmill, I make the radii R0.3" or so. In the toolpath this allows the tool to roll through the corner smoothly rather than making an abrupt direction change - less chance of chatter.

3. Be aware of feature depth. Generally the shorter tool you can use, the better. If you're designing a pocket, think of the ratio of length to diameter that the tool is going to use to get in there and mill it out. Ideally I'd keep this ratio less than 2.0, and definitely less than 3.0 if you want to be able to take heavy cuts at high rates.

4. Supply a well-made print with dimensions and PROPER TOLERANCES.

Again, really no substitute for experience... and a lot of subtle changes have a big impact. In 2004, the CNC'd uprights on our car took about a week or more EACH to make - because of design features, lack of machining experience, and running on crap machines. By 2007 with my redesign they were down to 1-2 hours each, and if I'd been a little more adventuresome it could have been much less. Then again, they were my personal carbide endmills bought on a college student budget, so I wasn't keen on breaking them http://fsae.com/groupee_common/emoticons/icon_smile.gif

If you do come up with a design, feel free to talk it over with machinists for advice on how to improve it. Or hell, post a picture here.

[RollingCamel]

We don't have any tools and machines available at our university so we went to a shop for $1550 for the uprights and $520 Al 6061 T6. While I wasn't responsible for its design, I had to redo it myself when the guy responsible was stupid enough not to put the caliper mounting's and bearing shoulder's plane perpendicular to the wheel axis. Thanks to the sharp eye of the machinist we were $2070 would have been wasted.

Anyways, we didn't think about the fixtures and it had to be repositioned so it took us more than a week to machine it, well they put some other work to machine in between because of their schedule.

Taking machining considerations into the design process is one of the most important things I learned from FSAE.

Thanks for the info.

[Jersey Tom]

One more thing that's good for part design in general - every feature you add increases cost... be it a pocket, fillet, hole, weld, chamfer, you name it. While they always add time and cost, they don't always add value or functionality. A good example are the people who feel compelled to fillet every hard edge they see, regardless of whether it makes a difference or not!

There is value in simplicity, even if it's on a CNC part.

[thewoundedsoldier]

@ Tom's #2:

I've come to desire the smallest diameter tool whenever possible. Both for the corner radius issue that you mention, and because the smaller the tool, the lower the SFM, meaning the faster I can feed. The exception to this is stuff like roughing and final pass. The trick here is to make sure that you keep your #3 recommendation satisfied.

I'd like to add that if you are both designing and machining parts, you should combine your efforts into using CAM software like MasterCAM. I'll "rough" design a part in Solidworks, then transfer it over to mastercam, then polish the design as I am editing the machine process. This let's me see how much time and effort I am adding to the process in real time, as I make changes. Then, once I am satisfied with the changes, I draw up the final part in Solidworks.

If you are just designing and not machining the part, then I agree with Tom that you should learn how to provide detailed, clear drawings with legit GD&T.