Use Work Features in Inventor, Part 1

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  Posted June 21, 2007

  by Community Admin1
  

  One of the most important areas to master in Autodesk Inventor 2008 is how to properly use work features in 3D modeling. Work features are defined as workplanes, work axes, and work points. When you properly create work features, they will remain parametric within your model or assembly and allow you to create complex geometry with ease.

  This first article in the three-part series on work features focuses on workplanes. Parts two and three will cover work axes and work points, respectively.

  Workplanes

  A workplane is a planar feature within most modeling systems. It is the primary work feature needed for creating extremely complex geometry. You may use a workplane for constraining parts or assemblies together, creating a new sketch on a non-planar face, as projected geometry in sketches, for measurements, or many other purposes. For reference purposes, Inventor creates three origin workplanes in every Inventor 3D file.

  In Inventor 2008, workplanes have a different color on each side to the workplane. The yellow side is designated as the "normal" direction, or the side in which the sketch will be created. To flip the normal side, right-click the workplane and select Flip Normal. Figures 1 and 2 illustrate the color change when the normal side is flipped.

  

  Figure 1. RMB – Flip Normal

  

  Figure 2. Normal (yellow side)

  Now let's take a look at how to create a few simple parametric workplanes on various parts.

  Create a workplane by vertices

  In our first example, we will utilize a simple model, and learn how to create workplanes through various points or vertices. (A vertex is described as an intersection between two edges, a midpoint of a single edge, a control point on a spline, or a placed work point.) You may create these models yourself, or download model files usable in Inventor versions 9 through 2008. Download Models9-2008.zip.

  1. Open the file -workplane1.ipt.
  2. Select the Workplane command.
  3. Select three vertices as shown in Figure 3. Yellow glyphs will appear when you are at a vertex.

  

  Figure 3. Select three vertices

  You will see a preview of the workplane. When the third vertex is selected, the workplane is created. (Figure 4).

  

  Figure 4. The workplane is created.

  Notice that the created workplane consists of a "blue" and a "yellow" side; the yellow side is called the normal side. If desired, you may flip the normal side by selecting the surface and right-clicking the Flip Normal command.

  Undo the workplane and proceed to the next example.

  Create a workplane by plane and vertex

  Using the same part, we will create a workplane through the middle of the part, parallel to the copper face. When a plane and a point are selected, the created plane will always be parallel to the original face or plane.

  1. Select the Workplane command.
  2. Select the copper colored face and then the midpoint of the top front edge as shown below (Figures 5 and 6). You will notice that the normal side of the workplane (yellow) is facing toward the original selected face.
  
  

  

  
  
  

  Figure 5. Select the face and vertex.

  

  Figure 6. The workplace is created (the normal side is visible).

  Undo the workplane and proceed to the next example.

  Create a workplane mid plane between parallel faces

  Using the same part, we will create a workplane through two parallel faces. This will create a workplane identical to the method above.

  Select the copper colored face and then select the face on the opposite side of the part.

  A workplane will be created midway between the two faces. If the thickness of the part is adjusted, the workplane will move to remain midway between the two faces. Be sure to pick Update to update the workplane position after any change.

  Undo the workplane and proceed to the next example.

  Create a workplane by two edges

  Using the same part, we will create a workplane through two parallel edges. The edges that we will select are the tangent edges of the forward facing vertical radius.

  Select the two vertical tangent edges. The workplane is now created and should be at an angle of 45° to the front face (Figures 7 and 8).

  Do not select Undo because we will use this workplane in the next step.

  

  Figure 7. Select three vertices

  

  Figure 8. The workplane is created.

  Create an offset workplane tangent to a face

  Using the workplane created in the previous step, we will now create a workplane parallel to the created plane or face and tangent to the front face of the radius. In addition, you can select an origin plane, then any curved face including the sphere, to create a workplane tangent to the object.

  Select the previously created workplane and then pick on the front curved face of the radius. An offset tangent workplane is now created. (Figures 9 and 10)

  

  Figure 9. Select the existing workplane and then face.

  

  Figure 10. The offset workplane is created.

  Be sure to pick Update to update the workplane position after any change in the model.

  Undo the workplane and proceed to the next example.

  Create an angled workplane

  You may create an angled workplane by selecting a line, axis, or edge and then selecting a parallel workplane or face. A dimension box will appear so that you can enter the desired angle as either a plus or minus number. A preview of the workplane to be created will appear so that you can easily judge the correct positioning.

  1. Using the Workplane command, pick a line or an edge, and then pick a planar face or existing workplane that will create a parallel plane.
  2. Input the angle in the dimension box (Figure 11) that appears. Figure 12 shows the finished workplane.
  
  

  

  Figure 11. Select Plane and then edge - angle.

  

  Figure 12. The angled workplane is created.

  Create a compound angled workplane

  You may create a compound angled workplane using the angle of workplane technique shown above and then create a sketch on that workplane. The sketch is used to create a second workplane at a compound angle.

  1. Create an angled workplane.
  2. Create a new sketch using the angled workplane. Sketch a line angled from one of the origin axis (Figure 13).
  3. Use the angled workplane and the sketch line from step 2 to create a second angled workplane at a compound angle (Figure 14).
  
  

  

  Figure 13. Create a sketched line on the workplane.

  

  Figure 14. Use the line/workplane to create the second workplane.

  Create a workplane at the end of a path

  If you are planning to use the sweep or the loft command in Inventor, you will need to create a sweep or loft path or paths, and then create a second 2D sketch at the origin of the path. The easiest way to accomplish this is to create a workplane that is perpendicular to the path and then create a new sketch on that workplane.

  1. Using 2D or 3D sketch, create a path for the loft or sweep.
  2. Select the Workplane command. Pick the endpoint of the path created in step 1 where you plan to place your profile sketch. After picking the endpoint, select the path line. The workplane is created. Be sure to flip the normal side of the workplane for proper sketch orientation. (Figures 15 and 16)
  
  

  

  Figure 15. Select the endpoint and then line/curve.

  

  Figure 16. The workplane is created at the end of the path.

  Use your imagination

  A great way to learn all of the ins and outs of creating and using workplanes is to branch out on your own and try different approaches to solving problems. Be sure to practice on all three files included in the downloadable zip file. I hope this tutorial will help get you started.

  By Dennis Jeffrey, AICE, MICE

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Comments

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  August 29, 2008 02:05 PM Rodney Keller

  Thank you for taking the time to write this article. Those new to Inventor will find it very helpful. I'll refer them to it.

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  June 21, 2007 05:46 AM Brian Hall

  Good Tutorial. Knowing workplanes and work features is a must when using Inventor.

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  June 21, 2007 06:46 AM Milton Rocha

  Great! These are the essential steps to work with Inventor.

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  June 21, 2007 06:46 AM George Bisanz

  Remember also that work planes aren't always necessary. Using model faces for new sketches instead of creating a work plane every time is a more efficient way to model. Users coming from AutoCAD sometimes equate UCS's with work planes, and create far too many of them.

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  June 21, 2007 01:20 PM Kody Baker

  Which one of these is new for Inventor 2008? Good tutorial on work planes, but I'm pretty sure they're all doable on versions up to v6 or so... The title leads one to believe that it will cover new items in Inventor 2008.

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  June 21, 2007 02:34 PM Dennis Jeffrey

  There are no changes to work planes. All versions pretty much have the same capabilities. This article applies to all versions. Any new items or options in this 3 part article will be noted in the text. The download files cover versions 9-2008.

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  June 29, 2007 01:30 AM Markus Schrepfer

  A very good article to basics of Inventor.