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JD Mather

Inventor 101

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JD Mather

EOP again.png

 

Drag the red EOP above the extrusion and fillet we just made.

(I just want you to get practice with moving the EOP.)

 

Start a new sketch on the top face of the part and sketch a horizontal like from the projected origin as shown.

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Sketch a rectangle as shown.

Do you know how to line it up symmetrically about the horizontal line?

 

Rectangle.png

 

Add a Coincident constraint between the midpoint of the vertical line and the endpoint of the horizontal line.

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Constrained rectangle.png

 

Dimension the rectangle as shown and then Extrude a distance of 8mm.

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10mm fillets.png

 

Fillet the 4 corners of the extruded rectangle with 10mm fillets.

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Drag the red EOP back down to the bottom of the feature tree.

 

add fillet.png

 

Edit the last fillet feature and add the loop around the bottom of the extruded rectangular feature as shown.

 

By moving the EOP up and down the feature tree we can manipulate how we add features and keep the number and type of features in a logical order that is easy to edit later.

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Start a new sketch on the top of the extruded rectangular feature.

Sketch a new rectangle as shown.

 

Hole Pattern.png

 

Convert or add sketch Center Points to the 4 corners of the rectangle.

 

Threaded Holes.png

 

Add the threaded holes as shown.

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Turn the part back over to look at the bottom.

As this will be a cast part - we need to add a draft angle to the 5 cylindrical features.

 

Draft 1.png

 

Pick the bottom planar face to define the Pull Direction and then pick the 5 cylinders.

 

Note: When selecting the cylindrical faces - pick then towards the bottom of the cylinders where they connect to the planar face. This connection is referred to as the "hinge".

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Finally, we need to add draft to the inside of the slot where we extruded an additional 8mm.

 

Draft.png

 

Pick the top face to define the pull direction and then click towards the bottom of the "horseshoe" face as shown.

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Paint.PNG

 

"Paint" the part by changing the part color.

 

Unpaint.PNG

 

"Unpaint" the machined faces by changing the Properties.

Remember - you can change a faces Properties by right clicking on the face.

Remember - you can change a feature Properties (like the Holes) by right clicking on the feature in the browser.

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Start a new Metric part file.

 

Start a new sketch on the XY plane.

 

Column Sketch1.png

 

Create the horizontal line going right from the Origin and the vertical line dimensioned as shown. Add three sketch points approximately a shown.

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Point Locations.png

 

Oops, I made a mistake on the location of the vertical line.

No big deal, simply double click on the 225 dimension and change to 240.

 

Dimension the location of the points as shown.

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Interpolation Spline.jpg

 

Connect the ends of the lines going through the 3 points with an Interpolation Spline (Notice that there are 3 types of splines).

After clicking the last point for the spline click the Checkmark or right mouse button select Done.

 

Add Tangent constraints between each end of the spline and the lines.

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Extruded Surface.png

 

Extrude the sketch midplane (symmetrical) a distance of 50mm.

 

Note: Because we did not have a closed profile - Inventor automatically extruded as a "surface body" rather than as a solid body.

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Next we will learn a new tool.

 

Thicken.png

 

Select the Thicken/Offset tool and set to Quilt, then select the surface body and set the direction and distance.

 

This is much faster than creating a closed profile. (especially where a spline is involved)

 

Save the file with the name Column.ipt

 

Turn the part over.

In the browser right click on the ExtrusionSrf1 and turn off the Visibility.

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Column Sketch2.png

 

Start a new sketch on the XZ plane and Project Geometry the edge shown.

Sketch a circle from the origin center point out to the edge of the projected line.

Finish Sketch and turn the part over.

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Extrude To.png

 

Extrude the circle To the top face as shown.

Be sure to put it to Join as Inventor will automatically assume you want to Cut.

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Slice Graphics.png

 

Start a New Sketch on the XY plane

Project Geometry the edge shown.

 

Hit F7 on the keyboard.

What happened?

Hit it a couple of more times.

 

Rotate the part around a little bit and hit F7 a couple more times.

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Three lines.png

 

Add three more lines - watching that Inventor automatically adds perpendicular or vertical or horizontal constraints as you go.

Dimension as shown.

 

Extrude midplane a distance of 180mm. (Note: when you want to Extrude you can simply hit the e key on the keyboard.)

Save the file.

Edited by JD Mather

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Start a new sketch on the XY Plane.

 

Rib Endpoints.png

 

Project Geometry the two points shown (you can either select endpoints or the edge lines themselves) (Tip: You should have Shaded with Edges turned on ).

 

Rib Sketch.png

 

Connect these two points with a line. Finish sketch and save.

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Rib Feature.png

 

Start the Rib command and set the parameters as shown.

Note that we can create a Rib feature with an open profile (single line in this case).

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