Matching contour flanges

[petercharles]

I have a conundrum! I have two contour flanges (straight – arc – straight) created from the same master sketch, one created “up” the other “down”. The intention was that these mate together on the common surface, and they do.

They will be laser cut from plate so I create a flat pattern for each part.

They need to be bolted together so need matching holes. My thought was to sketch on the top surface of the bottom flange and the bottom surface of the top flange using the Project Flat Pattern. I would then create a hole then pattern it, specifying the same pitch and number of holes on each part. They would then be “Cut” with “Cut Across Bend”. The holes line up on the first straight but start to drift once on the curve.

Any suggestions as to how I might achieve matching holes in the two flanges?

I’ve also noticed that when getting the Extents from the Flat Pattern the two lengths are different, the lower flange being 3315.93, the upper being 3340.29. But in the model they match exactly at the beginning and end. This rather confuses me!

Can anyone clarify what is going on?

[petercharles]

Did this end up in the "VERY HARD", or "IMPOSSIBLE" box?

[Anonymous]

> Did this end up in the "VERY HARD", or "IMPOSSIBLE" box?

Sorry, can't help with the hole transfers but (if I'm getting the picture, maybe
post one?); nested controured flanges will be different (developed at approx mid
thk) lengths.

[petercharles]

A common feature for us is bolting together two curved flanges, or more particularly flanges that are straight-curved-straight. You know, you take a couple of pieces of RS flat, drill them, then put them through the rolls. Now we've got Inventor we want to laser cut them complete with holes then just roll them.

I've used a master sketch and derived the two flanges (one 'up' and one 'down') from it and in an assembly they look great. But the holes are the problem. I don't seem to be able to get them to match up.

I've attached a ZIP file containing the master sketch, upper and lower flanges and an assembly. If anyone can help with this problem I'd appreciate it, as at the moment I'm into 'faking' it where I'd prefer a solid solution.

[Anonymous]

The dumdum box.
Buy using a master sketch that lies between the 2 parts… you’ve created the parts with 2 different form radii.

[petercharles]

Nope...

Just checked the parts in my ZIP file, the inside radius of the upper flange is exactly the same as the outside radius of the lower flange.

That's what we need for them to bolt together.

Anyone else?

[Anonymous]

Still not sure (no pic, no longer do drugs or IV) I'm correctly envisioning what
you are doing. A curved lap joint? If you understand (?) why the flat lengths
differ you should understand why holes, incorrectly laid out on the flats, won't
match.

I'm wondering, though, if you really want to do that. Are your fit tolerances
loose enough and fab tolerances tight enough to make it a practical idea?

[petercharles]

This is an arrangement we do all the time. We're talking about plates 3 to 10 mm thick. Since you can't see my IV parts here's a picture of a simplified asssembly. In practice because this one is a relatively short arc and there aren't many holes it's more easy. However in many cases the arc can be 90 degrees with a radius of 2000 mm and holes at 150 mm pitch. Thats when we get the problems that we need to fix.

Of course we could go back to the old ways, let the guys on the shop floor mark out and punch one part, then use that as a template for marking out the other. But that's not really why the management spent all this money on IV. We're expected to be able to create DXF flat profiles to go straight to the laser for cutting.

This stuff is also bespoke so we also need to be able to change the lengths and angle quickly and reliably which is why I'm going down the route of basing everything on a master sketch.

[Anonymous]

If you want to place the holes in the flat pattern (rather than in the finished
part and then flatten?) you could do is using a pitch correction factor derived
from curve on face and curve on bend neutral offset lengths.

[Anonymous]

“Nope... Just checked the parts in my ZIP file, the inside radius of the upper flange is exactly the same as the outside radius of the lower flange.”

Yep…

The common radius is the inside of the upper part, and the outside of the lower part. That means nothing to bend allowance which is calculated from a neutral plane somewhere between the inside and outside of the each material thickness. When you use a common sketch for the holes, and use “cut across bend” to put them in the formed part… your actually telling where to put the holes in the FLAT part. Then IV applies the bend allowance by projecting those holes to the neutral line of the folded part. If you create a IDW and over lay the FLAT parts you see the holes line up perfectly, but the parts are different lengths. Because, as I said before, you have 2 different form radii… Creating 2 different bend allowances.
Form radius being the same as inside radius. You do see that the inside radius are different. Right?

[petercharles]

Now I see it.
Doesn't help with putting the holes in though. I'm working on a method, but I don't know how easy it will be to impliment.

[Anonymous]

“Doesn't help with putting the holes in though.”

You had a 2 part question... How and Why
I think Why is usually more important to learn. For example...

Why I’m not going to tell you How.

[petercharles]

Well, now I can put the holes through both parts so they line up. Could be easier, but it's a solution.

[Anonymous]

This is less than 15 minutes of work..

Goodluck!

--
T. Ham
Mechanical Engineer
CDS Engineering BV

Dual Pentium XEON 2.2 Ghz
2 GB SDRAM
NVIDIA QUADRO4 700 XGL (Driver = 77.18)
18 GB SEAGATE SCSI Hard Disc
3Com Gigabit NIC

Windows 2000 Professional SP4
Autodesk Inventor Series 9 SP4
Autodesk Inventor Series 10 SP3a
--

wrote in message news:5103131@discussion.autodesk.com...
Well, now I can put the holes through both parts so they line up. Could be
easier, but it's a solution.

[petercharles]

Teun,
Thank you for your response which I have now looked at.

Unfortunately, my constraints are that the end holes are 150mm in from each end and the remaining distance is filled with holes at 150mm pitch from one end plus a makeup pitch.

As has been pointed out, I need to apply a correction factor to the pitching on the curve, plus a bit for the top flange, minus a bit for the bottom flange, so when you put them together the holes line up to get the bolt through. (although as a steel erector once told me years ago, "boy, if you can see daylight you can get a bolt through!")

I have a method but it's a bit of a pain and I can't integrate it to automatically change when I change the master sketch. But I'm not giving up yet .....

[Anonymous]

For the holes to line-up, the pitch of the holes in the bottom flange MUST
be different from the pitch of the top flange.

But the SkeletonPart is using the "common" line between the parts, the line
where the holes must line-up, so you will automatic get your correction
factor.

You can't specify one pitch which both flanges will use.

--
T. Ham
Mechanical Engineer
CDS Engineering BV

Dual Pentium XEON 2.2 Ghz
2 GB SDRAM
NVIDIA QUADRO4 700 XGL (Driver = 77.18)
18 GB SEAGATE SCSI Hard Disc
3Com Gigabit NIC

Windows 2000 Professional SP4
Autodesk Inventor Series 9 SP4
Autodesk Inventor Series 10 SP3a
--

wrote in message news:5103499@discussion.autodesk.com...
Teun,
Thank you for your response which I have now looked at.

Unfortunately, my constraints are that the end holes are 150mm in from each
end and the remaining distance is filled with holes at 150mm pitch from one
end plus a makeup pitch.

As has been pointed out, I need to apply a correction factor to the pitching
on the curve, plus a bit for the top flange, minus a bit for the bottom
flange, so when you put them together the holes line up to get the bolt
through. (although as a steel erector once told me years ago, "boy, if you
can see daylight you can get a bolt through!")

I have a method but it's a bit of a pain and I can't integrate it to
automatically change when I change the master sketch. But I'm not giving up
yet .....

[Ken]

Attached is a sketch of a method I've used to mate holes in mating sheet metal parts simiar to what you have. Basically I made a sketch of the mating flanges and made user parameters calculate the distances between holes on the neutral axis. I then use these values to layout a "flat" part. You can then make a flat layout from there if needed. Possibly you could adapt something similar to layout your curved flanges.

PS: Sorry about the pencil sketch. I can still think faster with a pencil at times. Can't say I've ever seen see anything this crude posted.

Ken Mozden - Tool Design
H-P Products, Inc
Louisville Ohio

[Anonymous]

Just wondering ....
Would it serve your purposes to blow the holes in as assy features, export the
solids and flatten?

[petercharles]

" .... to blow the holes in ..."

When I saw that phrase an image of one of our service engineers with an oxyacetylene torch in his hand came to mind!

[petercharles]

That's effectively where I am at the moment. I've established a correction factor that I can apply to my basic hole pitch. You add it on in the outside flange and take it off in the inside flange. Of course it's only to be applied on the holes in the arc not the straight portions and that's the bit I'm working on now. Maybe a VBA macro?

Alternatively I could just say "sod it" and change the holes to slots!