Post Split woes

peter_cuthbert

Good evening Everybody

Fired with enthusiasm after designing, drawing and getting 3D printed some parts for a custom stick holder on my whife's wheelchair I thought that the problematic ducting from the cooker hood should have the same treatment.  Of course life turns out to be rather more difficult than hoped.

I have now created a duct (See URL below) which I have sliced in half.  The reason for that approach is that the duct is in a cupboard and two halves with fins (or a flange) that can be bolted together makes the most sense for ease of fitting.  My difficulty is how to create the fins/flance on the curving surface.  Thus any pointer on how to tackle that would be greatly appreciated.

https://cad.onshape.com/documents/106320c74f44f08fcd2cfa7b/w/49777a555e2dda862a0eafaa/e/3e7ebabd0e9ee04d3c5956ff

Regards

Pete

nick_papageorge073

1) Change your approach from a loft to a sweep for the basic pipe shape. It will be way cleaner, and simpler to draw also. You would just need two sketches: the bottom circle, and the center sweep trajectory.
2) Once you have the basic pipe shape, go back to the circle sketch and add some ears on each side of it. Then go back to the sweep and grab those ears so it sweeps them along.
3) Split the whole thing down the middle, and in the middle of the ears.

nick_papageorge073

Here is an example.  https://cad.onshape.com/documents/06bb1d5e82b5c702080d531b/v/983a92a64b4d0a6624892192/e/2e35dbc1621b43804215558e

matthew_stacy

@peter_cuthbert, @nick_papageorge073 is right to recommend a sweep for this application premised on the assumption that you intend to maintain constant cross-section (diameter in this case) throughout the length of this duct.  LOFT, is a more generalized tool that blends multiple cross sections together.

I stuck with your Loft-based method, but made a few tweaks along the way.  Here is an example.

In my opinion, the symmetry of this part begs for a MIRROR rather than a SPLIT but either way works.  Frequently it makes sense to define variables for any dimensional value or parameter that will be used more than once.  Wall thickness (t) and flange length (L) are examples. 

For this particular loft, "guide curves" are far more valuable than a "path".  Smooth surfaces are built from smooth curves.  In general, use as few spline points as possible.  I chose to use zero intermediate points.  Those curves are controlled purely by the offset between your loft profiles, the orientation of the "end manipulators" (perpendicular to profile) and their length (I made all four equal in length, but that is somewhat arbitrary). 

 

Notice that end conditions for the Loft (normal to profile) match the tangency of the the guide curves.

Onshape has a sketch tool to offset curves (or any entity actually) that works well to sketch your flanges (of length #L).

Be sure to fillet the edges where flange meets duct before shelling.  Also note that the flange extrusion depth and shell thickness are both driven by the same variable #t.

These duct halves will likely prove challenging to fabricate in prototype quantities (presuming metal).  It is something that would probably require a highly skilled "tin knocker" (artisan with an array of hammers and anvils) or expensive stamping dies.

peter_cuthbert

Thank you Nick and Matthew for your wise suggestions.

That bronze duct looks magnificent compared with the bent and bashed corrugated ali duct that is there now.  I will press on and edit the drawing as you suggest though I wonder if the small distance between top and bottom may be part of the source of my problems.  I supsect that bending a 120mm duct in that space may well be pushing the limits. I might try going for an 80mm duct with 120mm end caps. My intention is to get this printed out on a 3d printer in ABS so if it can be drawn satisfactorily then it should be possible to print it.

Best wishes

Pete

peter_cuthbert

Thank you both.  I have now gone back and done a sweep which produces a very noce looking pipe (See attached)

However, when one adds the 'ears' to the base profile the loft falls over because the very sharp angles leads to self-intersection.  I think that I will undo the Shell, do a Split and then using the plane on which the split is based extrude that face as in your suggestion Matthew.  I can then Shell afterwards.

I am really beginning to appreciate how there are many ways to achieve a particular objective!

Regards

Pete

bryan_lagrange

Are you looking for something like this:

https://cad.onshape.com/documents/71a6d9500367baa2cc7c7d3f/w/16b7456643506a5d830fa393/e/31a4b4d5008832d5c00aacf1

peter_cuthbert

Hi Brian and fellow draughters

Yes, that is exactly what I was aimimng for.  I have managed to get that sort of effect, though I must investigate to see how you got yours.  My effort is here:

https://cad.onshape.com/documents/106320c74f44f08fcd2cfa7b/w/49777a555e2dda862a0eafaa/e/3e7ebabd0e9ee04d3c5956ff

What has made the drawing difficult is that the two connector centres are really quite close together so that getting the bends into the available space is not easy.

Having drawn it, I sent the file to a number of 3d printing firms all of whom said that the file was too large.  I then separated the two halves and re-saved them as separate files but got the same result.  There were a couple of firms that could cope with this size but their prices were out of this world. £200 or more for half a duct is not on my agenda.

Plan C is to find a way to cut the duct in half the other way and build in a connection mechanism.  Nothing has grabbed my enthusiasm just yet.

Regards

Pete