Quantcast

CNC cutting, tolerances and sheet metal assembly questions

HomeBuiltAirplanes.com

Help Support HomeBuiltAirplanes.com:

Arfang

Well-Known Member
Joined
Aug 10, 2014
Messages
98
Location
Switzerland
Good day all,

I'm trying to get a better understanding on sheet metal construction. As I understand, from looking at build logs and videos, rivet holes on the wing skin are drilled after being temporarily fitted on top of the ribs to make sure they're aligned with the holes already drilled in the rib flanges (or the other way around?) Same for fuselage skins, I saw people using some thin cardboard to get the accurate dimensions before cutting the skin panels. A considerable part of the assembly seems to follow the 'fit on assembly' principle. Is my interpretation correct? Could someone share ressources, be it personal experience, books, videos or websites to better understand sheet metal riveted construction? I already have Standard aircraft handbook and Sheet metal building basics, but I still struggle to fully understand the proper building and assembly sequence.

While I still have a lot to learn about sheet metal, I am familiar with milling, turning and designing metal parts with CAD which makes me choose metal over wood and composite. Plus I recently realized how left-handed I am working with wood. But I always worked with geometric dimensioning and tolerancing and trying as much as possible to avoid things like 'fit on assembly'. So, I had this idea of having all the parts cut and rivet holes ''drilled'' using a CNC cutter, be it laser, water jet or other, then flanging and riveting everything together.

The workflow would look like this:
Design in CAD, transfer the files to the cutter, cut and drill extrusion parts while the sheets are being cut, get the parts delivered and bend where necessery , assemble the entire thing. 90 percent of the aircraft is done, now you only have the remaining 90 percent to go.

Is CNC cutting all the parts, rivet holes included, a viable option, or standard practice? What level of accuracy would be needed to make it work? Assuming I have access to a CNC cutting machine and cost is not a concern.

Now my next concern is bending, like flanges on the ribs for instance. Let's say I got my parts all cut and drilled delivered, now I need to create flanges. What level of accuracy can one achieve forming flanges on ribs for instance? I remember seeing a video showing a way to create ribs using a hydraulic press and some MDF dye. Seems that this method would be able to provide a high level of repeatability. Are there other comparable methods and what would the largest part size you could practically use?

Are there any bending and assembly aspects that would prevent using pre-cut and pre-drilled parts?

As always, any help, suggestions and thoughts are appreciated.
 

rv7charlie

Well-Known Member
Joined
Nov 17, 2014
Messages
825
Location
Jackson
Aluminum designs have been everything from 'start with mining the aluminum' to probably 90% of the holes in both skin and underlying structure being pre-punched to size.

Current state-of-the-art kits like Van's RV12 have the holes punched to finish size, so all that's required for, for instance, wing assembly, would be to flute the rib flanges (to straighten the ribs) between the holes, debur the edges and holes, cleco everything together, and start pulling rivets. This obviously requires effectively perfect forming dies for the ribs, to get all the holes in all the ribs to wind up in the right places. I suspect that will be a tall order using MDF and a home shop hydraulic press.

Other kits (including RVs) have ranged from no holes, to holes in skin only (used as guide and match-drilled to the ribs), to matched holes but punched undersized (RV8 & RV7), so slight imperfections in hole layout and/or forming can be taken out with final drilling.

The 1st 'matched hole tooling' homebuilt design that I'm aware of was the Thorp T-18, designed back in the early 1960s. No CNC back then (at least not for homebuilders), so the technique was to use a drill template/guide. I've still got one lying around here somewhere. Builder would form all his ribs over a form block using a lead 'slap strap' (no hydroforming either).Then after creating his drill guide manually on a long strip of aluminum by laying out the rivet spacing, the guide is 1st wrapped around each rib ('inside' to the rib) and holes are drilled to match the template. Then, after laying out the spanwise rib spacing on the skin, the template is laid on the skin, 'outside' of the template on the inside of the skin. Holes drilled in the skin. Now the builder has 'matched holes' between skin & structure, and can cleco together and rivet.

Many, if not most, of currently produced kits include some level of CNC'd sizing and punching. A lot of them are *very* complete, as I mentioned earlier. Once the CNC code is perfected, it's gotten pretty cheap to run the stuff through the machines. And the current crop of builders tend toward the 'instant gratification' end of the experience spectrum, so it drives the kit companies to dance close to the legal max the FAA will allow them to prefabricate in a '51%' kit.

If I were just starting out and wanted basic info to get started, my 1st call would be to EAA. They will have books on everything from basic metal working to a lot more sophisticated techniques.

Charlie
 

proppastie

Well-Known Member
Log Member
Joined
Feb 19, 2012
Messages
4,636
Location
NJ
All of the above....depends on what you are building....basically unless you have a newly designed aircraft and kit such as a RV you will be "drilling at assembly" ... to assure the holes will line up.....and yes you can drill one piece first and match drill to the part under or drill both at once. The T18 has a technique for matched hole drilling pre CNC but most plans built or "materials kit" aircraft do not use it. You will want to cut large and trim later as to the skin. I would guess you would have to bend to +-.005 if you want to pre-drill say a rib and as was said above you probably would need hard tooling. If you have only one rib profile perhaps a drill jig after bending would work assuming your CNC router is good to 005 and your cad data is good....that is a lot of scrap if not.
 

Jay Kempf

Curmudgeon in Training (CIT)
Lifetime Supporter
Joined
Apr 13, 2009
Messages
4,008
Location
Warren, VT USA
If you make holes pilot holes you can allow the tolerance of drilling up to the final size in your accuracy. CNC hole patterns unto themselves are pretty accurate. So a row of rivet holes on one part is going to line up near or perfectly. The devil is in the bending and wrapping of the sheets. If you get your own CNC router that is made of aluminum extrusions and you have a pretty good handle on fixturing you can get really good accuracy. And if the machine is off a little bit it will be off the same each time so matching holes will line up. Back to bending as the devil in the details. If you wrap a leading edge for instance and your material is slightly more rigid or thicker than plan then you will have variability in length between the opposite edge holes. If you are adept with CAD you can build some test assemblies all the way to holes and then adjust your methods before cutting the real stock. Make one rib a piece of spar a leading edge section and the rest of the trailing edge. Make a flap or aileron a couple inches worth. Cheap insurance.

I'm going through the learning curve on composites right now. CNC in your shop is a whole new world.
 

proppastie

Well-Known Member
Log Member
Joined
Feb 19, 2012
Messages
4,636
Location
NJ
I see you are from the land of Metric +-.005 in. was what I meant . +- .13mm
 

proppastie

Well-Known Member
Log Member
Joined
Feb 19, 2012
Messages
4,636
Location
NJ
If you have access to a computer controlled bending break for your spars make sure you calculate your hole locations, bend locations based on the "neutral bend line" ....for large radius bends for aircraft that would be 1/2 T (thickness).....many of the newer cad programs have a "sheet metal" module which may calculate the blank and hole locations accurately.....The neutral bend line does not stretch or compress so the locations are based only by the geometry of the neutral bend line. Makes doing hand calculations of blank size or locations easy when you understand that.
 
Last edited:

proppastie

Well-Known Member
Log Member
Joined
Feb 19, 2012
Messages
4,636
Location
NJ
One gotcha with drilling holes in flanges before they are formed is that the holes themselves can stretch or shrink if the flange is curved.
although the latest completely match hole RV are drill/punched to size I would be undersized and drill to size at assembly to account for minor inaccuracy.
 

MadRocketScientist

Well-Known Member
Joined
May 16, 2009
Messages
1,623
Location
Canterbury, New Zealand, Earth, Milky Way Galaxy.
although the latest completely match hole RV are drill/punched to size I would be undersized and drill to size at assembly to account for minor inaccuracy.
That's what I did with my build, drilled all the holes 1/16" on the CNC and then to size on assembly. I left the curved flanges plain and drilled them in place using the predrilled holes in the skins as guides. It doesn't take much misalignment when folding parts to shift the holes. The smaller 1/16" holes can cover for a fold line being slightly off.

Getting the holes to match exactly is a lot of work for a one off. In a production environment, the form jigs and parts can be tweaked over several iterations to get everything to line up.
 

Jay Kempf

Curmudgeon in Training (CIT)
Lifetime Supporter
Joined
Apr 13, 2009
Messages
4,008
Location
Warren, VT USA
That is the best way. Pre-drill in the outer layer part, next to go on and use it as a drill jig. The one thing about pre-drilling flat sheets like the RV is that you can debur on the bench in the flat and if lucky put it together once. I think I read that RV bought a half million dollar Amada and everyone thought he was nuts at the time. He proved them all wrong. Punch presses are FAST and can be very accurate if programmed properly (which I did in a past life, on 8 bit tape!).

Take a look at Cheapracer's build thread. He is moving into CNC drilling matched parts and designing an airplane from scratch to use flat wrapped shapes that will still be a quite low drag airframe. Take a look at the BD-4. This is another flat wrapped airframe suited to pre drilled holes. Very low drag for what it is.
 

Rik-

Well-Known Member
Joined
Sep 13, 2019
Messages
399
Location
San Rafael, California
In nearly all CAD programs today, you can draw your shape, layout your holes and the use the "Tool" "Make flat" which as it says will take that curved shape and give you the accurate representation of what flat sheet of material is needed to make that curved shape.

With this "Flat Shape" you have merely send it to a job shop with a cnc punch press and punch out the holes and or laser cut the entire panel out.

Then once you bend the flat panel to shape the holes will be perfectly laid out.
 

Jay Kempf

Curmudgeon in Training (CIT)
Lifetime Supporter
Joined
Apr 13, 2009
Messages
4,008
Location
Warren, VT USA
Yeah, kinda. If the shape was curved before you flattened it the holes won't be round anymore. If you didn't account for the bend centriod (testing and adjusting) the holes won't line up. So you tweak. There are sheet metal bending parts of some CAD systems that will account for all that stuff. But again you have to adjust to actual real world conditions. Sometimes the way things are bent it is all stretch and the inside surface is the actual layout. Sometimes not. So you tweak and adjust the bent factor to make it work. BTDT, have the T shirt been to the seminar and the school of hard knocks on all that. Done it in 2D drawing board, 2D CAD, 3D CAD, parametric, programmed the machines, tested the assemblies.
 

proppastie

Well-Known Member
Log Member
Joined
Feb 19, 2012
Messages
4,636
Location
NJ
half million dollar Amada
usually punched holes have a break and micro cracks but I have been told Van uses "zero clearance punch and dies" and this is not a problem.....If you send out your cad to a shop you may not get the zero clearance punch and die so it probably is best to punch undersized.
 

rv7charlie

Well-Known Member
Joined
Nov 17, 2014
Messages
825
Location
Jackson
For decades Van's told us builders the story that the punch/die causes shear lines in the hole edges (it does) which are stress risers that are removed by the drill when final match drilled. Then the -12 came out with final sized holes, and they said that they could get away with it because the -12 uses pulled rivets, which don't expand into the hole and stress it like a bucked rivet (that's true). Then the -10 came out with largely final-size-punched holes, and....Crickets.

If you examine a CNC punched hole with a magnifier, and then examine that same hole after you've 'reamed' it with the final-size drill (the standard process) and deburred it with a (relatively common) 3-flute deburing tool, you'll likely have a coronary at the damage you've done with the drill & 3-flute debur tool.

What does AC43 say about using a Whitney Punch? (Same process; just not CNC controlled...)

Charlie
 

Arfang

Well-Known Member
Joined
Aug 10, 2014
Messages
98
Location
Switzerland
Thank you all for your answers.

I would guess you would have to bend to +-.005 if you want to pre-drill say a rib and as was said above you probably would need hard tooling. If you have only one rib profile perhaps a drill jig after bending would work assuming your CNC router is good to 005 and your cad data is good....that is a lot of scrap if not.
By ''bend to .005'' do you mean the linear distance between flanges? How would you achieve that on a rib with a curved flange for instance?

Regarding the hydraulic-MDF board method, are there more accurate methods to do a curved bend, not necesserely available to the average homebuilder but in general? All I'm aware of are bending presses to do straight bends.

That is the best way. Pre-drill in the outer layer part, next to go on and use it as a drill jig. The one thing about pre-drilling flat sheets like the RV is that you can debur on the bench in the flat and if lucky put it together once. I think I read that RV bought a half million dollar Amada and everyone thought he was nuts at the time. He proved them all wrong. Punch presses are FAST and can be very accurate if programmed properly (which I did in a past life, on 8 bit tape!).
That's the kind of machine I had in mind.

So the main problem seems to be punching holes in flanges before bending because there's deformation during the process that's difficult to account for and would require extensive trial and error. Plus the CAD software can't convert the part to a flat pattern since it's not flat-wrapped anymore.

If I understand properly, the easiest way to have rib flanges drilled is to use some kind of jig after forming or to drill using the skin holes as guides. Here's my question: if let's say the ribs are drilled using the skin holes as guides, what reference point do you take and how do you precisely position the skin panel on the ribs?

Another question, what are the typical tolerances for rivet holes in diameter and between two holes? If I take the Amada ACIES-2515B for instance, it has an accuracy of plus-minus 0.1 mm or .005 inches, which would result in two parts potentially having .01 inch between holes centers.
 

Jay Kempf

Curmudgeon in Training (CIT)
Lifetime Supporter
Joined
Apr 13, 2009
Messages
4,008
Location
Warren, VT USA
Amada we used to get .005 between holes but you have to look at the whole hole pattern. If the clamps slip you loose the whole part. We had what was called an auto-index station or two to do the exterior nibbling with a small rectangle or obround. Wear is an issue. Diameters were to tenths of a thousandth of an inch. But wear of the tool is an issue especially with small tools. Tight tolerance dies can create really nice square holes but they can't go as fast and they wear out faster and jamb more. Everything is a compromise.

A good CNC router can do all you need and just robotically drill holes and position to say .001 across feet of travel. Routers don't move the sheet and for small thicknesses you can choke up on the bit and get really good hole size and position. Not as fast as a punch press. But you can do other things while it runs.

Best way I have found to position holes on flanges around even a complex part is to position the holes from the edge and then adjust the flange bend depth to compensate. Works quite well. Did acres of galvanized commercial appliance stuff that way. Prototype, adjust once then run off acres. Holes dead on every time. And we didn't have windows then only DOS. Remember DOS?
 

rv7charlie

Well-Known Member
Joined
Nov 17, 2014
Messages
825
Location
Jackson
There are milspec and FAA documents for hole sizing, pitch, edge distance, etc etc. All pretty well defined now.

The typical way to 'match drill in place' the ribs to the skin is:
Establish rib centerline spacing on the main & trailing edge spars, and duplicate that spacing for the lines of holes in the skin. Lay out the holes in the skin for spars' flange attachment.
Punch/drill all the holes in the skin.
Draw a centerline (extra-fine Sharpie for precision) on each rib flange, and a line on the spar flange to match.
Rivet ribs to spar web, and to the trailing edge spar.
Jig the skeleton so that the main & trailing edge spars are in correct relationship to each other, in both both square and twist.
Lay skin over the ribs, and align the leading edge of the skin with the correct line on the spar flange..
Pick a starting point on the spar near the center-most rib, at the spar, and align the intended mating holes in the skin over the lines on the spar and rib, making sure rib is square to the spar flange.
Drill 1st hole and cleco.
Verify that everything is square and aligned along the spar, and drill/cleco another hole in the spar flange, a foot or so away from the 1st hole. This locks the skin in alignment with the spar.
Now each rib can be flexed to align its centerline under the holes in the skin.
'Work your way back/out from the starting point, drilling & clecoing.
The ribs will try to flex & move around; they're just prodded into position for each new hole.

You can get most of this kind of info, in much better detail, if you purchase a set of plans for an older metal homebuilt line a Midget Mustang, Thorp T18, etc.

Charlie
 

proppastie

Well-Known Member
Log Member
Joined
Feb 19, 2012
Messages
4,636
Location
NJ
By ''bend to .005'' do you mean the linear distance between flanges? How would you achieve that on a rib with a curved flange for instance?

Regarding the hydraulic-MDF board method, are there more accurate methods to do a curved bend, not necesserely available to the average homebuilder but in general? All I'm aware of are bending presses to do straight bends.
When I say bend to .005 I mean the tolerance of the part after bending is +-.005 which includes the hole locations. and I am not talking hole to hole location but rather absolute location of each hole. As to how you achieve that in a curved part ....you need proper tooling. When I say hard tooling I mean at least aluminum forms for a hydro press with location pins to fix hole locations or male female steel dies.....These dies have to be developed by skilled tool makers to give you a part that meets tolerance every time. Forming a rib with flutes so it is flat is a more difficult/expensive tooling problem.....Cheap racer designed his ribs with notched tabs for the flange which is easier to form.
 

proppastie

Well-Known Member
Log Member
Joined
Feb 19, 2012
Messages
4,636
Location
NJ
True, but with a $20 pair of fluting pliers the builder can address that in just a minute or two per part ;)
agreed but Op wants to drill in the flat bend and have matched hole parts.....a much more difficult problem. When I worked at McDonnell Douglas even they did not have matched hole skins and ribs....most everything was fancy fixtures to drill at assembly. There was matched hole tooling in WWII for some parts when Ford and GM were building aircraft as I understand it.
 
Top