Inventor - Engraving on a sphere

[220610]

Hi,
I've been looking around and couldn't find a solution. I have a sphere which I'm able to project on a sketch of smaller circles which I'd like to engrave over it's surface, yet I want each of them to be perpendicular to the surface of the sphere in each point. Emboss doesn't do the trick, it just makes the engraving perpendicular to the plane.
Can someone please help?
Thanks!

[JDMather]

Solution in this document or attach your file here.

http://home.pct.edu/~jmather/SkillsUSA%20University.pdf

[220610]

Ok, it partially worked.

I've tried using "adjust" to correct, and chose the starting point, and while it does "stick" them to the surface, it doesn't "correct" their orientation, which should be perpendicular to the surface.

Here's what I mean.

[JDMather]

You also have to set the Direction 1 orientation.

But there are other problems - starting with Sketch1 unconstrained.

I recommend going back through your part and constraining the sketches.

No 3D sketch needed and you are not ready for 3D sketches.

I will come back in a bit and walk you through solution.

[220610]

Ok, I've repaired the unconstrained parts. I've deleted sketch1 as it was obselete.

This is after constraining, and still the same problem occurs.

I'm not sure what you mean by "You also have to set the Direction 1 orientation.", I thought I did.

I'll wait for your reply.

Thanks a lot!

P.S.

Not sure how I got so caught up in this tiny problem, as I already did something (which I believed) more complicated, an Uzi SMG with movement constraints and all.

[JDMather]

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220610 wrote:

P.S.

Not sure how I got so caught up in this tiny problem, as I already did something (which I believed) more complicated, an Uzi SMG with movement constraints and all.

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Unfortunately - I'll wager it was all wrong too.  Time to learn proper Inventor techniques.

BTW - you did not set the Direction 1 Orientation.

[JDMather]

Before I spend a lot of time on this - are you willing to spend the time? Do you want to learn how to model correctly?

This angle is not manufacturable and because of the way you dimensioned the arcs are not concentric and therefore the wall thickness is not 5cm. (only those two lines are 5cm)

[JDMather]

Start a new part file.

Set your units to cm if not already set.

Create Sketch1 as shown and attach the file here.

[t22e]

I'm willing to learn to do it properly, a good foundation is the most important thing.

You probably guessed it already, but I learned the program by myself and on the move, so that's where my faulty methods are from.

I anticipate our difference in time zones will make delays in our correspondance, so I apologize in advance.

Thank you for doing it.

I'll do everything you sent and will send the files back once it's done.

[220610]

Hmm... logged me before as guest, nevermind, I'll sort it out later.

Ok, so I've done as you said, I think, that's why they're are two files. 

One of them is bound to be what you did (I really hope, otherwise I'm in a bigger hole than I imagined).

Thanks again!

[kvannj]

I think he means that you should make only one sketch (in 2D), make a centerline (not construction), and simply draw a normal line and set the dimension to Ø120. When you set a dimension to a centerline, you get the diameter directly and not the radius.

[220610]

I more than certain you're right, but for some reason it doesn't switch the normal line (drawn from the centerline) as a diameter

[JDMather]

Neither file you attached looks like what I posted in image, so we will take this one step at a time..

Create a new sketch on the XY plane and then create a vertical line from the origin (I turned on the center point so you can see) and dimension it 30mm.  Save and attach the file here.

[JDMather]

Select the line and then click Centerline in upper right corner of screen (on standard install).

Save and attach your file here.

[JDMather]

Create a horizontal line from the top of the vertical line.

Then Dimension by selecting the free endpoint of the horizontal line and the Centerline (not endpoint).

Enter 120 as the dimension.  This should result in a diametrial dimsion.

Save and attach your file here.

[220610]

Thanks for the detailed explanation, there's hope for me yet!

[JDMather]

Edit your sketch and create a Center Point arc.

Click anywhere on the centerline except for endpoint or midpoint to constrain the center of the arc to the centerline.

Then click the origin and then in space for the 3rd point.

Drag the free end of the arc to the end of the horizontal line.

Then R OK. (to Revolve)

Then Shell and select the planar face and enter the shell thickness.

[JDMather]

Start a new sketch on the XY plane and then hit F7 (I also went into wireframe visual style).

Create the sketch as shown. 

If  you constrain the "top" of the hole to the inside curve - be sure to use the outside point rather than the centerline point.  (or you could go all the way out to the planar face.

R - Cut OK (to Revolve Cut).

[JDMather]

Get lazy - use geometry constraints rather than dimensions.

Create the sketch shown on the XZ plane.

Then do your Extrude Cut (do you really want a planar face on the bottom of this extrude or do you want it curved like the outer face of the part)?  Do you want the sides with no taper angle?

[JDMather]

I forgot a critical step - go back and edit the sketch for this feature

Project Geometry the outside spherical curve (must be projected before the Revolve Cut).

After exiting the edit sketch - right click on the sketch in the browser and select Visible.

[JDMather]

Notice also that in all my images I had right click on the Origin Center Point in the browser and turn on it's visibility.

When you do your Curve Driven (Rectangular) Pattern be sure the Start Point is at the origin and be sure, be sure, be sure to set the Orientation to Direction 1.