Aerospace Machined Part Design, Producibility, etc... 2

[IrishBob]

I am new to aerospace structural design and will be designing a lot of machined parts. My employer has plenty of info on cutter radii, etc, but little in the way of design manuals for machined parts and I would like to know if any of you can point the way to any good books or websites that might help me.

I'm mainly interested in tips on how to design pad-up transitions, machined joggles, radius blends, etc. For example, the CAD system we use (CATIA V5) will produce different filleting results depending on the order in which I pick the edges and I'd like to know which is 'correct'.

A website with pictures of 'good' machined parts would be cool as well.

Thanks in advance. Learnt tons from this website about airplanes thus far...

 

[40818]

If your create machinings for aircaft, then the parts should comply with the whatever OEM your working for.
Say your doing machinings for Airbus, then you have their proceedures to follow etc.
What you can and cant produce will entirerly depend upon the machining technolgy your company possesses; you could design something that required a double sided machining using 5 axis and requires a weeks to scan that costs £X0000, or you could have a simpler design that isn't so fancy but could be knocked out in no time and costs relativley peanuts.
Speak to your chief designer and ask him/her for guidance or company literature.

 

[IrishBob]

I know what you are saying but while we get told what cutter sizes to use by the mfg group, thicknesses supplied by the stressman and the mfg guy claims they can make 'anything' (regardless of cost, though) our producibility guy is nowhere to be found so I am looking for a little external guidance.

I may be green, but I am not ignorant so I do know what makes one machining more expensive than another (1 or 2-sided, open or closed-angle, etc). In the auto business you could find a real part to look at but here.....

One thing I am finding is that cost-of-manufacture appears to be a buzzword in Aero. In my recent Auto experience it was the opposite - quality took second place to cheapness.

 

[40818]

Your right with the quality issue. It is paramount, because when i do my analysis it is based upon (amongst other things) its geometry. If the geometry is outside of the allowed tolerance the part requires me to have a look at it and either concess the part or scrap the part, either option costs time and money, i know of whole wing spars being scrapped due to problems and 6 figure losses.

 

[ferdo]

Hi,

I saw this

http://www.omwcorp.com/partdesign.html

in another forum.

Its not quite you are looking for, but I hope will help you a little bit.

Regards
Fernando

 

[KENAT]

Aerospace takes quality more seriously than most, I worked in airborne weapons so combine aerospace & explosives, imagine how tight quality was.

As regards the radii CAD puts in. Think through what the likely cutter path will be and this should usually help.

I was gonna lead you to the same linke as ferdo so I'm waisting my time now.

KENAT, probably the least qualified checker you'll ever meet...

 

[Kwan]

Just some more info:

Note: i am not aware of any web sites. I learned more about producibility by reading the various company's design guidelines. Well, more from the producibility engineer and talking with the mill operator.

Consider a bathtub fitting. Corner radii would be generated by the radii of the tool or tool path, fillet radii is at the bottom of the bathtub.

Manufacturing wants a large corner radii, small fillet. Stress analysis typically wants a small corner, large fillet. Manufacturing rule would be no more than a 4 to 1 depth to diameter to minimize tool bending. Another consideration to to keep the corner radii slightly bigger than the cutter. This keeps the mill from "banging" into the corner; thus, reducing stress on the mill.

I think you also talked about minimizing set up (one sided machining, etc). Always try to fully understand how the shop will acutally set up the mill for each cut. I usually start my models with a solid block (same size as raw stock) and cut the part as a mill would. This give you a great understanding of the process. Also, this will produce a more precise model. One method I've used is to create surfaces, then use them for the cuts. This method works great in joggles/steps. Otherwise, a portion of the model contains a radii that requires an extra cut by the mill (sometimes).

Then you have to consider residual stress. One sided milling could be detrimentally affected by the residual stresses. Thus, machining cost are reduce. However, scrap might increase.

It's a balancing act with every design. You are the hub of a wheel. Stress, manufacturing, management, etc are the spokes. Just stay in the center if you can!

Anyway, I believe your best bet is to talk often with the mill operator and the producibility engineer. Hopefully I helped a little.

 

[ferdo]

Hi,

IrishBob, if you want even more informations, search also CATIA forum on this web site or repost this thread there.

You will find a lot of useful things, speaking from CATIA user point of view.

All the info mentioned here are very useful also.


Regards
Fernando

 

[KENAT]

Kwan give some good advice, especially on modelling.

For machined parts I too usually start with a 'block' and cut parts away. This helps think about how manufacturing may make the part.

For a lot of these things different shops/machinists etc will say different things.

Some excerpts from our design manual:


a) Avoid designs requiring sharp corners or points in cutting tools - they break easier.
b) Avoid thin walls, thin webs, deep pockets or deep holes to withstand clamping and machining without distortion.
c) Avoid tapers and contours as much as possible in favor of rectangular shapes.
d) Avoid undercuts that require special operations and tools. Design around standard cutters, drill bit sizes or other tools.
e) Avoid hardened or difficult to machine materials unless essential to requirements.
f) Avoid small holes and threaded features that can cause tool breakage and part scrap that will increase costs.
g) Design for minimum full thread depth. Usually 1.5 X major diameter provides adequate holding strength. Avoid the requirement to tap to the bottom of blind holes, use minimum full thread call out when possible.
h) When material thickness allows, thru holes are preferred.
i) Counter bores should be used in preference to countersinks whenever possible.
j) Chamfers should be used instead of radii on external features. (some debate on this with CAM)
k) Radii should be used on internal corners instead of chamfers.
l) Always specify largest radius possible. Small diameter tools add significant cost to manufacturing process.
m) When depth exceeds 5 X the diameter of the pocket radii, consult selected vendor on alternative fabrication methods. Depths of up to 10 X are possible when machining aluminum but not all manufacturing facilities have that capability.
n) Design composite curves, such as internal pockets or other profiles, such that CNC manufacturing will have a continuous cutting path. When possible the radii should be constant to allow the use of the same cutting tool. Design for and specify unilateral tolerances (+/- .010). Reason: This allows size control variation of the features being machined without having to control the NC program (file) to an exact match with the cutter diameter.
o) Design tolerances should be within manufacturing capabilities and the maximum possible while maintaining design integrity.
p) Concurrently designing for manufacturing will greatly improve product quality and reduce fabrication costs. Consult with selected machine shop early in the design process. After completion of preliminary drawings, meet with manufacturing and review design intent, requirements and determine manufacturing process requirements. Manufacturing should review tolerances and determine process capabilities to meet dimensional limits. Manufacturing should identify tolerance challenges that require design and requirements review. In general, design should avoid unnecessarily tight tolerances that are beyond the natural capability of the manufacturing processes. Determine when new production process capabilities are needed early to allow sufficient time to determine optimal process parameters and establish a controlled process.
q) Tolerance stack-ups should be considered on mating parts. Overall assembly tolerances should be calculated, to determine interface clearance requirements.


KENAT, probably the least qualified checker you'll ever meet...

 

[tbuelna]

IrishBob,

Depending upon the application or usage of the finished part, things like allowable mismatch at blends, surface finish, stress relieving, heat treating, edge breaks or even how the part is handled during machining can be very critical. Especially if the part is fatigue critical and/or subject to fracture control. As many posters have pointed out, the contractor will usually require you to work to their process procedures and will also require QA documentation to prove that you have. And don't expect them to look the other way if you miss even something minor. Writing DR's costs them money, and if they refuse to DR the part, your company's going to eat the cost.

Most subcontractors for the major aerospace OEM's must be certified by that company before they'll be given any work orders. They must also have additional QA certs like AS9100 before they're even allowed to bid on jobs. The big aero companies take this supplier certification very seriously, and they're constantly monitoring their suppliers for conformance. As a supplier, if you end up with too many non-conformance issues on the parts you deliver, you will likely lose your certification for doing business with that company.

Of course, all of the certs in the world won't guarantee timely contract performance by your subs. Boeing just proved that with the 787 program.