Attaching an object to a curved surface

[srjacob]

I have completed my snoot (thanks to all the help here), and I am trying to attach two objects to the slanted surface.

What I did was copy the original sketch and pasted it into a new sketch, which caused the new sketch to overlay the original (non-rotated) outline, then drew my new object on that, and rotated it slightly, then did a circular pattern to the the object to other side of the snoot. I have attached my drawing file to show how what I did. Fortunately, what I did worked.

There has got to be a better way to do what I did, and I am hoping some of you more experienced mavens can show it to me. If the surface was curved (instead of slanted), I'm not sure how I could have accomplished it.

I'm not a newbe at Alibre, I just haven't done this before.

For anyone's curiosity, this snoot goes on the business end of an Xrite i1 to get spectrum and intensity of 5mm LEDs. I have written some custom software that does the computations. The objects in question hold a rubber band to hold the snoot onto the i1.

 

[wazzu83]

A couple of observations. Your approach is sound. However, your sketches are not fully constrained. This can & will lead to many problems.

I offer an alternative approach. I used measurements taken from your sketches & model part.

See attached.

 

[HaroldL]

Use Project to sketch to convert sketch<1> into reference figures in sketch<2>. Then fully constrain sketch<2> and you're set.

 

[idslk]

1) i also vote for fully constrained sketches (min. is fixed constraint)
2) two configurations only to show 2 additional ways maybe for other "events"...



Regards
Stefan

 

[srjacob]

A couple of observations. Your approach is sound. However, your sketches are not fully constrained. This can & will lead to many problems.

I offer an alternative approach. I used measurements taken from your sketches & model part.

See attached.

wazzu83: I took a look at your part file, and when I tried to edit the sketches to see what you sketched, the edit was grayed out and I couldn't see what you did. How do I un-gray the edit?

 

[srjacob]

A couple of observations. Your approach is sound. However, your sketches are not fully constrained. This can & will lead to many problems.

I offer an alternative approach. I used measurements taken from your sketches & model part.

See attached.

I copied your file to a separate directory and I could edit the sketches. However, how did you do sketch 2 and project it onto the surface?

 

[wazzu83]

I copied your file to a separate directory and I could edit the sketches. However, how did you do sketch 2 and project it onto the surface?

Apologies ... try changing the color of the part to a lighter color. You probably can't see the sketch because my fully constrained sketch objects are gray.

1) I inserted Plane<3> @ distance 22.31 mm above YZ-Plane (same distance as measured in your model to top face of your "object"

2) Sketch<2> on Plane <3> is a pair of concentric 15° arcs of radii measured from your model (r1= 20.959 mm, r2=18.95 mm) enclosed the arcs with radial lines.

3) Extrude To Geometry, selecting surface of cone Face<3> as Target Geometry.

4) added Fillets

5) Revolved Feature Pattern

 

[srjacob]

Apologies ... try changing the color of the part to a lighter color. You probably can't see the sketch because my fully constrained sketch objects are gray.

1) I inserted Plane<3> @ distance 22.31 mm above YZ-Plane (same distance as measured in your model to top face of your "object"

2) Sketch<2> on Plane <3> is a pair of concentric 15° arcs of radii measured from your model (r1= 20.959 mm, r2=18.95 mm) enclosed the arcs with radial lines.

3) Extrude To Geometry, selecting surface of cone Face<3> as Target Geometry.

4) added Fillets

5) Revolved Feature Pattern

Ahha! The key is extrude to geometry. I didn't know it would extrude to a non-planar surface.

 

[HaroldL]

when I tried to edit the sketches to see what you sketched, the edit was grayed out

A hint for you and anyone downloading files from the forum. IF your browser download setting is set to Open the file in Alibre then do a SAVE AS and save the file where ever you choose. The Edit function will then become active and available.

Also, for the single sketch you could also have selected to extrude To Next, just make sure it's in the correct direction. I lke the To Next option since I don't have to select any geometry, just let Alibre do the work. One thing that is a bit odd about To Next is that it only works with single loop sketches and multiple loop sketches will error out with the status message that states "Disjoint loops not supported for To Next extrusions".