Inventor 101

[JD Mather]

Start a new Standard(mm).ipt part file.

 

Select the YZ plane in the browser and right mouse button New Sketch.

 

 

Sketch the Polygon as shown (what do you have to do for it to be fully constrained)?

Tip: Remember - when not fully constrained - drag endpoints should give you a visual indication of what you need to do.

If, after dimensioning and dragging an endpoint - you still don't understand what needs to be done - I recommend that you change majors. Geometry is not for you.

 

Exit the sketch and save the file as M6 Hex Head Bolt.ipt

[JD Mather]

Start a new sketch on the YZ Plane.

 

 

Project Geometry one of the lines from Sketch1 into our current Sketch2.

 

Sketch a circle from the origin Center Point out Tangent to the projected line.

 

In the previous image note that there were two black lines in the sketch.

These were the Horizontal axis (Thick) and the Vertical axis (thin). I prefer to turn these off as they clutter up the screen. Next we will do some of this "house keeping".

 

Finish Sketch and save the file.

[JD Mather]

Well, I'll do the house keeping later, but notice that I keep changing the background color. I will get around to showing you how.

 

 

Find the red End of Part marker in the browser.

Drag the red EOP marker above Sketch 2 and notice that Sketch 2 disappears from the graphics window. At any time we can move back in history by moving the EOP to complete an operation we forgot. In other words, Inventor is like a time machine.

[JD Mather]

 

Extrude the hexagon a distance of 4.7mm as shown.

[JD Mather]

 

Drag the red EOP marker back down below Sketch2.

 

 

Extrude the circle through All with the Intersection option (remember this one from the Table part above)? Almost no one knows how to use Intersection - welcome to the professional world.

 

 

Click on the More tab and set a taper angle of 45°. Click OK and observe the result on our geometry.

[JD Mather]

Turn the part around.

 

 

Right click on the face shown and select New Sketch.

Sketch the circle shown and then Extrude it a distance of 10mm.

[JD Mather]

 

Add a 0.5mm Chamfer to the end of the cylindrical extrusion.

 

 

Click on the Thread tool.

 

 

Click the cylindrical face for the location and then -

Set the thread Specification as shown.

Save the file.

[JD Mather]

I promised some "house-keeping", let's get it over with.

 

Go to Tools>Application Options and make the following changes. (these screen captures were taken from 2015 - if using a different version - your screens might look slightly different)

 

 

On the Part tab. Set as shown.

 

 

On the Colors tab. Set as shown. I recommend using either the Sky background or the Image Millenium2 background.

 

 

On the Sketch tab. These are the most important settings. Make sure you get these exactly like mine (both the on and the off).

 

 

On the Assembly tab. This will help when we get to assemblies.

[JD Mather]

On the Navigation bar at the right side of the screen.

Click on the little black arrow in the bottom right corner.

 

Oops, looks like we did this earlier.

 

 

Select Visual Styles

 

 

Set to Shaded with Edges.

Edited April 24, 2014 by JD Mather

[JD Mather]

Be very careful on the next couple of steps.

 

Open the file M6 Hex Head Bolt.

 

Save As M8 Hex Head Bolt.

Verify at the top of your screen that you are now editing the file M8 Hex Head Bolt.

 

Right click on the Thread feature in the browser and select Delete.

 

Expand the Extrusion1 and right click on Sketch1 and select Edit.

Double click on the 10mm dimension and change to 12mm. Finish Sketch.

Right click on Extrusion1 and select Edit Feature and change the distance from 4.7mm to 6mm.

 

Expand Extrusion3 and right click on Sketch3 and select Edit.

Double click on the 6mm dimension and change to 8mm. Finish Sketch.

Right click on Extrusion3 and select Edit Feature and change the distance from 10mm to 40mm.

 

Start the Thread tool and click near the end of the bolt (not near the head).

Uncheck Full Length and change Length to 20mm.

 

Save the file.

[JD Mather]

Save As the file with the name M18 Machine Screw.

Next we will learn how to cut a physical thread. (on the previous examples we created a simple "cosmetic" representation of threads - just a picture)

Physical thread are useful for 3D printing parts (cosmetic thread will not 3D print).

 

Delete the Thread feature.

 

Edit Sketch1 and change to 27mm.

Edit Extrusion1 and change to 10.7mm.

 

Edit Extrusion2 and change the Taper angle to 60°.

Edit Sketch 3 and change the 8mm to 25mm.

Delete the Chamfer feature.

 

 

Edit Extrusion3 and change the distance to 0.8mm.

Save the file.

 

 

 

I'll be back.

[JD Mather]

Start a new sketch on the face shown of a circle Ø18 and Extrude a distance of 70mm.

 

[JD Mather]

Go to the Front view and start a New Sketch on the XY plane.

 

 

Project Geometry the top horizontal edge of the cylinder as shown.

 

 

Sketch a Polygon triangle as shown (be sure to use the Polygon sketch tool).

Add a Horizontal constraint to the top line of the triangle.

 

 

Click and drag the left top corner of the triangle to the end of the projected line and then dimension as 1.5mm (NOTE: if use a version of Inventor before r2014 dimension the line as 1.4999 (it will show rounded as 1.5).)

 

 

Finish sketch and then add a 1mm Chamfer to the end of the cylinder.

[JD Mather]

Yesterday we left off with our part ready to cut the thread.

 

Go to the Coil command.

 

Select the X-Axis as the axis of revolution and flip the axis direction.

Set the output to Cut, then...

Go to the Coil Size tab and set to Pitch and Height from the drop down list.

(Why you are in that drop-down list, what is the very last option? That is a "hidden" option that very few are aware of. Commit it to memory if intend to take the Certification exam at some time in the future.)

 

Set the Pitch to 1.5mm and the Height to 42mm. Click OK.

 

Remember - you can set colors/textures by Part, by Feature, or by Face.

Right click on the Coil Feature and set the Properties to some other color.

Change the part Material to Steel and the Part color to Chrome.

[JD Mather]

Lets finish it off to look more realistic.

 

Start a new sketch on the triangular face of the end of the thread.

Select Project Geometry and click in the middle of the triangular face.

Notice in the browser that projecting a face results in a Projected Loop.

I usually recommend to NEVER project a face as a loop, but in this case the triangle will not change - so it is OK.

Go to Coil, set to Cut and with a Taper as shown.

 

Save the file.

Now Save As with a new name Table Post.

[JD Mather]

Delete the two Coil features in the Table Post part.

Delete Sketch5 in Table Post.

 

Right click on the Fillet feature and select Edit Feature (or you can double click on it).

Change the 1mm Fillet to 0.5mm

 

Edit the 70mm extrusion and change to 27.75mm distance.

Edit the 18mm sketch diameter and change to 11.875mm

Edit the 0.8mm extrusion and change to 26.25mm

Edit the 25mm sketch diameter and change to 15.875mm

Edit the Extrusion1 and change the distance from 10.7mm to 8mm

Edit the Sketch1 and change the polygon dimension to 18.

 

Your part and feature tree should now look like this.

[JD Mather]

 

Start the Hole command and set the placement to Concentric.

 

Select the end face of the cylinder and then the side of the cylinder.

Set the parameters as shown.

 

Save and close the Table Post file.

[JD Mather]

Oops, I forgot some features and need to change the order of operations.

No big deal. Re-open the Table Post part.

 

 

Click and drag the Chamfer feature to below the Hole feature (or conversely - click and drag the Hole Feature to above the Chamfer feature).

 

Notice that we can change the order of features as long as we don't try to move a child feature before it's parent. In this case, the Hole is not a child of the Chamfer, but the Hole feature is a child of Extrusion4 and therefore cannot exist before Extrusion4. This is simple logic. You cannot exist before your parent.

[JD Mather]

 

Now that we have moved the Chamfer to below the Hole feature, right click on the Chamfer and select Edit Feature.

Add the edge of the Hole and the edge of Extrusion3 to the Chamfer feature as shown.

 

Now save and close the file.

[JD Mather]

Start a new Standard(mm).ipt file.

 

Start a new sketch on the Top Plane.

 

 

Sketch a rectangle oriented approximately as shown (offset) from the origin.

Add the angled line from the origin to the midpoint of the left vertical line.