Archive for November, 2009

Round parts and features… Part 1

November 30, 2009

Features, and Holes on cylindrical parts, or How do I draw on Round things…? PART 1

As we all know, round parts have a slight sketching challenge; there are no planes to pick from the cylindrical surface. This can be a problem if one is not aware of the tools provided; a combination of construction planes and axes to allow feature definition on the cylindrical surfaces. These include angle offset, offset from the center axis, and various other positional locations on a cylindrical part.

Let us take a look at some solutions and tools to help with these tasks. Note the figure below represents a part that could become a problem child:

A working knowledge of Planes and Axis tools will be needed to define any of the holes and features in the part above.

TIP:  turn on your default work planes…

Starting with the raw part below:


Let’s add a feature to the part like the particular one identified below…

Adding the hole feature is very easy and straight forward, and we will use the point & line technique to define a sketch plane on the cylinder surface.


1. Drop a plane along the part Axis at desired location…

2. Create a new sketch on the plane created in step (1)

3. Create the vertical and angled line as shown above, and then dimension to the desired angle as show in figure below. This will provide us with the ability to rotate the position of our feature around the part cylinder and along the length of the cylinder – two positioning controls!

4. After finishing the sketch from steps 1, 2 & 3, use the line created in the sketch to create a plane on the end point of that line and normal to that line. The figure below shows the expected results…

5. Now we need to select the plane just created as our new sketch plane, add the geometry to define the hole (feature) shape, see the figure below…

TIP: if this is a counterbored hole, define both the counter bore dia., and the hole dia. in this sketch and share it later for the hole creation.

Hope you found this process helpful. The following PARTS of this TIP sheet will cover the creation of the remaining features each using a different process…

Stay Tuned


iPhone and Inventor

November 13, 2009

Ok, for all you iPhone users out there, you may have already seen Sketchbook, the handy little application from Autodesk.

Well, here’s a nifty video showing how you can incorporate those sketches you produce on a lazy Sunday at the bar into Inventor.


11-13-2009 3-19-08 PM


Vertically-centering text objects in Inventor drawings.

November 12, 2009

When creating drawings in Inventor, you may want to have text center (middle-justify) vertically. The problem is that the preview looks great, but the text will not center in the drawing.

wc text justify 1

Here are the steps to change files that have an existing justification problem:

General step 1: Make a copy of the current drawing’s annotation objects style & edit the copy…

wc text justify 2

The reason for making a copy of the style is twofold:

     1) The original style is preserved without change. This makes it easy to revert back.

     2) A style can be copied & modified more than once to create easily customized objects.

General step 2: Use the copied & modified style to set the defaults for the desired drawing objects…

wc text justify 3

General step 3: Select annotation object(s) to be modified (hold <Ctrl> key down for multiple selections) & change their style from the drop-down list…

wc text justify 4

Any type of annotation object can be modified using this procedure. Simply set up the desired style or standard parameters in a copy of the existing style/standard, then use that style as the default for individual objects in the “Object Defaults” section of the dialog box. That’s it!


Showcase Subscription Advantage Pack

November 12, 2009

For all you lucky lucky people out there with Showcase and Subscription, check out the Subscription Advantage Pack here:

There’s some fantastic additions to the feature set, my particular favourite being the keyframe animation capabilities. 

Takes the product to a whole new level.

Have fun.


Mixing and Stripping with Inventor

November 12, 2009

Have you ever tried mixing your units in Inventor parameter equations?

For example, you have a pattern of features which you would like to change depending on the length of a part:

stripping units 1

You may have tried something like pattern_qty=length/2

Because length has units of inches and pattern_qty is unitless, the equation will turn red as Inventor does not understand the concept.

stripping units 2

The trick is to strip the equation of its units by multiplying length by 1ul/1in.

So, in the example shown the equation should read pattern_qty=(length*1ul/1in)/2.

Or, if you would like to round the resulting value down to the next whole number, then:


stripping units 3

Have fun.