Loft Error: "Cannot use faces or regions with inner loops as profiles

ode_tujoy

Hi, I'm building my first Onshape part and having a hard time creating a loft from extrude to thicken. Is this possible? or did I take the wrong approach.

This is a leaf blower adapter for an EGO electric blower. It attaches to the round end of the blower and extends to a 45 with a "stadium" exit nozzle. 

Not sure how to share the direct link but the document I'm working on is called EGO Blower adapter

robert_scott_jr_

Right click on your document's URL and copy it to the clipboard. Select the link icon to bring up it's dialog and paste the copied URL into it.

I've come across the same message myself. Although I can't explain why, rest assured there is a reason Onshape does not allow the selection but there are methods to accomplish the task.

Please post a link as I am currently modeling and printing parts for my EGO blower nozzle to accommodate round corrugated downspout as an extension for gutter cleaning. I'd like to see what you've got going.

https://cad.onshape.com/documents/247d06d6a6c1e4b5b8ba406a/w/41ed2a3440f896a505de76c9/e/ff0116672d7a375842ae1af4

- Scotty

glen_dewsbury

Hey Robert
I recommend starting your object from the origin. That will simplify down stream features and eliminating adding more planes. The mate connector becomes unnecessary as well since any circular edge  of solid or sketch can be selected for circular patterns.
The inside cut outs I made are not based on your sketch but are a how to suggestion. I don't recommend using a continuous spline for the inner cut out. To many control points needed. Looks like you eyeballed the spline into place. 
Is the split done to be able viewing inside? If yes, look up section view for clarity and select one of the planes.
https://cad.onshape.com/documents/cab81f14d3d41ffcc5b2a7ed/w/1dc4bf84898121b513a6c850/e/b1e152cce9ecce53ffaba4f1

robert_scott_jr_

Hello Glenn. I agree about using the origin as a place to 'fix' a point in the sketch. The shape I started with was irregular and I tried to find some center for it but couldn't really identify any. Probably should've used the transform tool later on once I had eyeballed centering the shape to the circle, fixing the circle's center to the origin. Due to the irregular shape, is there an alternative to the continuous spline? Using multiple splines and intersecting their ends?

The splits were required due to resin printer limitations (gonna fix that someday).

Thanks for your input.

- Scotty

ode_tujoy

hopefully this link works for you all

https://cad.onshape.com/documents/a2c5e91cd6616f5711f330d9/w/47ad6de25105531a48228532/e/9fe9ea77fe1c262e166a4287

glen_dewsbury

Here is a sample to use a series of Bezier Splines that I find easier to control. Make sure that the end handle of one is parallel to the next for tangency and don't let unwanted constraints get in there. Hold shift key to prevent auto constraints. Don't add anymore points to the Bezier curves than needed as this will make it harder to control and poor transition across surface connections.
You'll need to find a way to get some control measurements to scale and place the BMP before tracing. I've eyeballed start points and fixed them so that when pulling spline handles so the whole thing doesn't pull out of position.
Figuring out placement and scale of BMP is kinda flaky and hardest to do unless you have the original part in front of you.
https://cad.onshape.com/documents/cab81f14d3d41ffcc5b2a7ed/w/1dc4bf84898121b513a6c850/e/b1e152cce9ecce53ffaba4f1
You can also rotate BMP if that helps.

glen_dewsbury

@robert_scott_jr_
I just realized you said down spout! You should be able to get these dimensions directly from the down spout with a cut out for the seam. That should be closer than the tracing of a BMP and will be to scale. Wrap a gear clamp lightly around it to steady the shape if needed. Measure up the tube a bit so your not dealing with a beat off end.

glen_dewsbury

@ode_tujoy
A simple way to accomplish the transition is to break up the circle so that it will the same number of edges as the rectangle. The loft is happiest when the number of edges is the same on each profile. There is another method during the loft build but I think this will suit your purpose. Loft does not like open profiles like the tube sections. That's why I did these as surfaces and thickened the whole thing at once. You can also loft as a complete solid then shell.
https://cad.onshape.com/documents/1826edd69b5ec6c2515a6fe4/w/eac3f934eaa4afee07b6605b/e/fc87cce01c5972677930cbab

matthew_stacy

@ode_tujoy, make your life easier by making Extrude1 and Extrude2 both solid or both surfaces.  I went with solids, then loft the faces of those two extrudes selecting "normal" (perpendicular) for both end conditions.

Then Shell the solid.

Model

ode_tujoy

matthew_stacy said:

@ode_tujoy, make your life easier by making Extrude1 and Extrude2 both solid or both surfaces.  I went with solids, then loft the faces of those two extrudes selecting "normal" (perpendicular) for both end conditions.

Then Shell the solid.

Model

Hey, thank you! I followed your advice and it worked like a charm. Made a lot more sense from a workflow perspective as I was doing it too. 

Secondary question related to this part. 
The cylinder portion (where this adapter will sleeve over the ego blower) is slightly tapered to match the taper of the blower tube. 
Does anyone have a goto tolerance for plastic/plastic friction fit? I've made a few test sections (just the cylinder part) and they're all really tight. Each section takes about 6hrs to print and a considerable amount of filament. Hoping someone had a cheater number they start with that is close.

The I.D of the tube at its narrowest is 3.5" with a taper to 3.55" at a distance of 3" 

Thanks for the help!