Autodesk® Inventor® and its Construction Environment

We all love getting something for free. When we buy a car, free usually comes in the form of a tank of gas or some floor mats. When we buy a computer, we typically get access to music websites and setup help for free. When we buy software, when it comes to the core code, we typically don’t get anything for free that can be used beyond 30 days without paying for it…or do we? With software, it’s a given, most of us do not use the full potential of the software. On average, we use 50-75% of the core software’s total abilities. So what’s in that ~25% area that we might be missing out on? In this article we’ll be covering the Construction Environment which is a piece of that ~25% area.

Now, for Inventor, that average usage of 50-75% only considers the core product and does not factor in any vertical modules such as Simulation, Plastic Injection Tooling or Pipe/Wire Routing. With that in mind, the Construction Environment (CE from here on because I’m that lazy when typing) comes as part of the Inventor base programming. There are many other little freebies in there similar to the CE such as Sheet Metal, Frame Generator, Design Accelerator, Studio, iFeatures, AEC Exchange, Assembly Substitutes, and Weldments, just to name a few (okay, all of them). Consider it an environment if the interface changes or it has unique commands that only relate to said operations, which is why I included iFeatures.

Okay, enough blabbering, time for the down and dirty info. The CE is for working with surface geometry, and bypasses the need for a history item in the tree. In other words, any changes made in the CE are not seen in the tree and can’t be modified after the fact, other than Undo. So, just a strong word of caution when working in the CE. Now, take a basic model that you might get via STEP or SAT or IGES or any format that opens as a surface entity –or– a solid entity. Typically, the surface geometry will come in as a Composite Surface, or group of Composite Surfaces, and the solid as a Base Solid. Either of these can be copied (notice I said copied) into the CE for editing. Simply right-click on the feature and you get a Copy to Construction choice. When this is chosen, the browser nodes will change to include a Construction folder (see Figures 1 & 2 for reference).

Figure 1 (Copy to Construction)

Figure 2 (Construction folder)

To access (activate) the CE, simply double-click on the Construction folder in the browser. Note, it is extremely helpful to disable the visibility of the original geometry *outside* of the CE before working in the CE. Inside the CE, the Inventor Ribbon menu (or tool panel in the class mode) will change to display the commands applicable to the CE (see Figure 3).

Figure 3 (Construction Ribbon Interface)

Each command listed obviously provides different functions and results and again, none of them will create a feature in the history tree. Let’s look at each of them, starting from the left.
Copy Object: Use this command to promote geometry *out* of the CE and back into the normal modeling environment.

Quality Check: Analyzes the surfaces for translation quality. A poor quality surface typically cannot be manipulated as much as a good quality surface.

Stitch: Essentially it sews everything together into one surface “quilt” much like grandma used to do with a patch-work quilt.

Unstitch: Separate’s the surface “quilt” into a separate surfaces entities.

Boundary Patch: Creates a surface patch by using connected edges (edges must be connected as you cannot string between two points to define an edge in the CE).

Intersect Faces: Allows two different options for faces at intersection. Either keep all faces and break along the intersection, or remove the surface extents beyond the intersection.

Boundary Trim: Trims a surface based on the connecting boundary of another set of surfaces. Different from Intersect Faces as it only works with one face to another face, whereas Boundary Trim will look at one face to cut, and multiple faces to build the cut profile.

Extend Faces: (can be mathematically intensive on the CPU) Changes the length of an edge or edges of a face to a given distance. If the input distance cannot be achieved, Inventor does a “best fit” calculation and extends the edge(s) as much as it can.

Edit Regions: Allows you to choose a face with openings and choose whether or not to keep said openings or remove them (patch them). Think of a flat surface for casting that has machined holes in it. Use Edit Regions to remove the holes by choosing to keep the flat face & the hole fill.

Extract Loop: Extract the wire edges of a surface or set of surfaces to use for trimming of surfaces.

Reverse Normal: Reverses the +/- of a surface. This can be extremely useful if the plan is to use that surface in the Offset/Thicken modeling command of the part environment.

When should these commands be used?
Let’s look at this scenario. In your business, you make casting tooling and you receive a finished part model in a different CAD format (see Figure 4 for reference). This finished model has some machined areas on it that you must remove in order to build a viable pattern impression. Notice the drilled holes, the machined “U” pocket, and some gaps in the surfaces, all of which will need to be corrected before extracting surfaces for tooling topology. Plus, this file translated over as a surface instead of a solid, which pretty much guarantees the need to use the CE to reconstruct the geometry.

Figure 4 (Casting Image)

So, step 1, rmb (right-mouse button or right-click) on Composite1 in the browser, select Copy to Construction. Now turn off visibility of the original Composite1 in the browser and double-click the Construction folder in the browser. Personally, I find it visually easier to work on surfaces that *are not* translucent - so rmb on Composite1 under the Construction folder and disable Translucent (see Figure 5).
Next, a Quality Check should always be done to test the validity and structural quality of the surface geometry. Even though this part translated into Inventor containing gaps in the surface geometry, the quality of the surfaces translated successfully and the Quality Check shows no issues. If you encounter surfaces that are deemed poor quality; the Quality Check utility will provide suggestions on massaging the surfaces into a higher quality.

Figure 5 (Translucence Control in the Construction Environment)

With the surface quality good, start by removing the holes. Select the cylinder walls of each hole and hit the Delete Key to remove the cylindrical surface. Next, use Edit Regions on any non-cylindrical surfaces and Boundary Patch on the cylindrical surfaces. Boundary Patch should be used on any holes that are split across two surfaces (See Figure 6 for reference).

Figure 6 (Edit Regions)

Use Boundary Patch to cover all other holes on the model. For the options inside the Boundary Patch command, changing to the Tangent Condition (See Figure 7) will yield better surface continuity of the patch against the surrounding surfaces. Continue using Boundary Patch to close the gaps in any surface geometry.

Figure 7 (Boundary Patch Tangent Option)

Once all patches have been built, run the Stitch command to build the surface “quilt”. Starting the Stitch command, rmb in the modeling area and choosing Select All is a nice lazy button to grab all surfaces for analysis. The preview shows all edges in red that can be successfully woven into a quilt of surfaces. See Figure 8 for reference.

Figure 8 (Stitch into “Quilt”)

Now it’s time for Copy Object. With a successfully woven “quilt” of surfaces, we have a lot of options when using Copy Object. Inventor gives us the power to work with surface geometry to build and edit solid geometry with ease; however, the vast majority of users prefer to work with solid throughout the modeling process if at all possible. With a quality “quilt” created in the CE, select the entire body of surfaces and a new output option shows up in the Copy Object dialogue box. You can promote surfaces back into the part modeling environment as a solid. You can also choose to “Delete the Original” CE geometry. See Figure 9 for reference.

Figure 9 (Copy Object Options)

Exit the CE and now there’s a Base (Solid) to work with. But wait a second, we forgot to fix that “U”-shaped machine cut while in the CE. We could have done that in the CE, but honestly, it might have taken more clicks. This is typical with some, what could be considered basic, model features that need removal. Since we have a quality solid object to work with, we can use one of the surface commands in the modeling environment: Delete Face. Delete Face can be used to select a single face or set of faces to remove, and if you click the Heal option, Inventor will attempt to remove the faces while also filling in the void with material. See Figure 10 (before) and Figure 11 (after) images for reference.

Figure 10 (before)

Figure 11 (after)

You now have access to the multitude of other Inventor commands along with Split and Derive to build the casting tooling from the customer supplied model geometry. This scenario looked at a casting situation, but this could apply to mounting tooling, reference hole locations, assembly clearance for fit or for use when Extruding or Revolving “To” a face or faces.

Inventor has a lot of little freebies like the Construction Environment that can help you work with non-native CAD data for your own workflow. The Inventor Help documents the Construction Environment very well and these tools are simple to use. However, should you need help, just call a Hagerman Sales Rep and ask how you can get help using or learning Inventor’s Construction Environment. We’ll be glad to help get you rolling into a new world of extremely powerful and useful tools.

Thanks to the engineers at James Thomas Engineering, Inc. (http://www.jthomaseng.com/jtehome.htm) for providing the part geometry that was used in this newsletter article.

This page last edited on Monday, February 14, 2011