Inventor General Discussion

Inventor General Discussion

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220610
Posts: 22
Registered: ‎12-01-2012
Message 31 of 48 (267 Views)

Re: Inventor - Engraving on a sphere

09-04-2013 12:35 AM in reply to: kvannj
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
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JDMather
Posts: 28,254
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Message 32 of 48 (258 Views)

Re: Inventor - Engraving on a sphere

09-04-2013 04:48 AM in reply to: 220610

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.

 

Line.png

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Message 33 of 48 (255 Views)

Re: Inventor - Engraving on a sphere

09-04-2013 04:51 AM in reply to: JDMather

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

Save and attach your file here.

 

Centerline.png

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JDMather
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Message 34 of 48 (254 Views)

Re: Inventor - Engraving on a sphere

09-04-2013 04:55 AM in reply to: 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.

 

diametral dimension.png

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Contributor
220610
Posts: 22
Registered: ‎12-01-2012
Message 35 of 48 (226 Views)

Re: Inventor - Engraving on a sphere

09-05-2013 06:15 AM in reply to: JDMather

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

 

 

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JDMather
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Message 36 of 48 (217 Views)

Re: Inventor - Engraving on a sphere

09-05-2013 08:09 AM in reply to: 220610

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.

 

Arc.png

 

Then R OK. (to Revolve)

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

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Message 37 of 48 (208 Views)

Re: Inventor - Engraving on a sphere

09-05-2013 08:35 AM in reply to: 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. 

Sketch2.png

 

curve constrain.pngIf  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).

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Message 38 of 48 (204 Views)

Re: Inventor - Engraving on a sphere

09-05-2013 08:46 AM in reply to: JDMather

Get lazy - use geometry constraints rather than dimensions.

 

Create the sketch shown on the XZ plane.

 

Get Lazy.png

 

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?

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Message 39 of 48 (201 Views)

Re: Inventor - Engraving on a sphere

09-05-2013 08:53 AM in reply to: 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).

 

Spherical Projection.png

 

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

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JDMather
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Message 40 of 48 (198 Views)

Re: Inventor - Engraving on a sphere

09-05-2013 09:00 AM in reply to: 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.

 

Orientation.png

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