Inventor 101

[JD Mather]

Start the Hole command (most of these commands can be started from the keyboard as well as from the Ribbon icons. E for Extrude, H for Hole).

 

 

Set the Hole for Concentric and then click the planar face of the part and then the cylindrical face of the part. Set the hole dimensions as shown and then hit OK.

Edited April 18, 2014 by JD Mather

[JD Mather]

Add the two 0.5mm chamfers as shown.

 

 

Assign Stainless Steel as the material (remember how to assign materials). (If you forgot how - see Post #15 - there will be a test on this stuff.)

 

Save the file.

Edited April 15, 2014 by JD Mather

[JD Mather]

Test 1 (I told you that you would be tested on this stuff).

 

 

Start a new mm part file and create this sketch on the XY Plane.

 

Fortunately - you get to use a "cheat sheet".

 

1. Sketch the horizontal line from the origin and change it to a Centerline.

2. Sketch the left vertical line from the origin and add the diametrial dimension. Do it now. Do not continue without the dimension.

3. Sketch the top vertical line and dimension the 10mm. Do it now. Do not continue without the dimension.

4. Sketch the right vertical line and angled line to the centerline to approximate size. Trim the centerline (new command we haven't done).

(Tip: Remember that you can click and drag line endpoints.)

5. Add the remaining diametrial dimension and then add the angle dimension by selecting the angled line, the centerline and then clicking where to place the dimension. These last two dimensions sometimes give beginners trouble (especially placing angle dimension). For the Ø3mm dimension you are dimensioning from the ENDPOINT of the angled/vertical lines to the centerline.

Edited April 16, 2014 by JD Mather

[JD Mather]

Double click on the Ø3 dimension and enter Punch_Dia=3mm and click the green checkmark.

Double click on the Ø3 dimension again and notice that is it now a named Parameter.

We will use this later to make something called an iPart (and intelligent part).

 

Finish Sketch and then Revolve the sketch around the centerline.

Change the material to Steel and save the file as Punch Die.ipt

[JD Mather]

Start a new mm part file.

Let's get fancy.

 

 

Sketch a circle at the origin.

But this time instead of going to the Dimension tool on the ribbon (or hitting d on the keyboard), click and drag the right mouse button down to the left to about the 7-8 o'clock position. Notice that the dimension tool appears at our cursor. Once you get good at this you don't even have to wait to see the tool - you can simply right mouse "gesture" to that position and get into dimension. In fact, once you get good you don't need to see most of the tools, you can gesture to what you want to do next.

 

Maybe that is a little too advanced for now - but start paying attention and practicing

[JD Mather]

 

Dimension the circle as Ø220mm and then Extrude a distance of 36mm "away" from us (Direction 2).

Save the file as Table.ipt

[JD Mather]

Start a New Sketch on the XY Plane (Remember how to do this? Right click on the XY Plane in the browser and select New Sketch).

 

 

Select the Polygon sketch tool and make sure it is set to 6 sides.

Click the origin center point as the first point and then approximate size as shown.

[JD Mather]

 

Select the Horizontal Constraint tool from the ribbon and then click the bottom horizontal line of the polygon (or any line). Adding geometry constraints like Horizontal, Vertical, Tangent..... is the key to Inventor sketching. As you get experience - Inventor will add nearly all of these constraints for you automatically, but beginners often struggle with this and see it as extra work.

 

 

Add the dimension across flats.

Notice that the sketch has changed color (your colors might be different than mine - we'll discuss that in a bit) and Inventor should report Fully Constrained.

[JD Mather]

Next is a professional trick that few make use of - Intersection options of features.

 

 

Select the Extrude tool and set to Direction 2, through All and Intersection.

 

This will find the intersection of our hexagon and cylinder leaving 6 flats on the hex.

Did something right? Save the file. Every time you do something right - save the file.

[JD Mather]

Click the arrow in the lower right corner of the Navigation bar on the right of the screen.

 

 

Then set the Visual Style to Shaded with Edges. I always work with this visual style. After we finish this part I will show some other settings that I change on the interface.

[JD Mather]

Right click on the planar face at the top of the part.

 

 

Select New Sketch to start a sketch on this planar face of the part.

[JD Mather]

Now we learn a new tool that is key to using Inventor sketching.

 

 

Select the Project Geometry tool and click the line at the back of top the planar face as shown. Later we will see that if we change previous geometry - this projected geometry will always update to reflect the changes made to previous (parent) geometry.

 

In other words - the solid we had before is a Parent of this projected edge which is a Child of the parent and therefore looks like the parent. Understanding Parent/Child relationships is the key to understanding Inventor. For some reason beginners have trouble with this, even though they have no trouble recognizing who their own parents are or recognizing who their own children are. If you are unsure of this (Inventor parent/child relationships or your own parent/child relationships) I predict trouble at some point in the future.

[JD Mather]

 

Sketch a line from the midpoint of the projected line to the point that was projected from the Origin Center Point (did you notice that point). That is the key to Inventor sketching (the projected center point).

 

Add a sketch point to the midpoint of the line you just created.

Exit the sketch and save the file.

[JD Mather]

 

Start the Hole feature command and notice that Inventor automatically selected our sketch center point as the location for the hole.

 

We want a flat bottom hole with the specifications shown.

Then click OK and save the file.

[JD Mather]

 

Start a new sketch on the XY Plane and sketch the circle and line shown. Dimension and change to Construction linetype. (Have we done that yet? Construction is just above the Center linetype.) Construction lines are the key to Inventor sketching.

 

Add the sketch point to the end of the line as shown.

 

Tip: Did you notice that I chose to select the XY Plane rather than the planar face for creating this sketch. Either one could be used, but if you have a choice - always use the Origin planes for sketches. This is referred to as the BORN Technique. Remember the Parent/Child relationship. The Origin planes have no parents and cannot be deleted, while the solid could be deleted or significantly changed - enough to cause trouble with our new sketch. We could lose information on who the real parent of the sketch is - if we depended on the solid geometry.

BORN = Base Orphan Reference Node The Origin planes and Center Point cannot be deleted - so if we use them as our parents - we won't be confused about who are real parents are at some point in the future. This is the key to Inventor modeling (or SolidWorks, or Creo, or....).

[JD Mather]

 

Exit sketch and start the Hole command.

Set the parameters as shown and then click OK>

Save the file.

[JD Mather]

 

Click the Circular Pattern tool from the ribbon.

 

With the Feature selection tool active select both holes we have created.

Make the Axis selection tool active and select the cylindrical side of the part.

Click OK.

Did something right? Save the file.

[JD Mather]

Start the Hole command again.

 

 

Next we make a counterbored hole at the center of the part with the parameters shown.

 

Assign the material Steel to the part.

Save the part.

[JD Mather]

Let's paint the cylindrical sides (faces) of the part.

 

 

Holding the Ctrl key - select the three cylindrical faces shown and then right mouse button select Properties.

 

We can control Properties by Faces, Features or by the part.

When we turned on the Shaded with Edges visual style we could see boundary lines of each individual face of the part.

 

If we right click on a feature in the browser (like say, Hole) we can change the Properties of all of the faces of that feature at one time.

[JD Mather]

 

Notice that if we change the part properties, the face properties still override the part properties.

 

Note there is a difference between Material properties (Steel) and part/feature/face properties of color/texture. A lot of beginners get confused by this, for example assigning a Brass color property, doesn't assign the brass material properties.