Whenever you import a third-party part model into Inventor, most of the time you end up with a featureless solid. Inventor over the years has improved the tools available to edit these solids either directly or in the creation of features from solid entities. Below is a SolidWorks part imported into Inventor 2016 using the AnyCAD application. The model is feature entity rich, but once imported it is a dumb solid to Inventor.
Among the solid editing tools are ones that will move, rotate, size, lengthen, delete, etc. the entities of the solid model. The focus of this article is to present a method of accomplishing the modification of an array within a solid. It is not a direct command but a combination of a few. The process can save a lot of time and effort. If you desired to change the patterned hole count around the center of the above solid, you would find out quickly that the pattern feature tool does not work since there are no (Inventor) features in the model. The most effective way to do this part is to simply delete the existing pattern add a new hole, chamfer it and then pattern to the desired count. But what if you had a solid where the pattern was made from a cutout shape not as easily duplicated. A example of this is shown below. Sure you could use the same method outline above but read on, maybe the process below will be easier.
The first step is to create surfaces from one of the triangular cutouts in the pattern. I will select the one facing one side of the plate. Creating surfaces from existing surfaces is quickly done using the "Copy Object" command located on the 3D Model Tab under the Modify panel.
Starting the command, I first make sure that I will be selecting faces not solids and that I will either be creating surfaces or composite surfaces, either one will work.
After selecting the three inside faces of the triangular cutout, select "OK" to finish. The browser shows the new composite (group of surfaces).
The next step is to close off each end of the triangular cutout with a boundary patch. The "Patch" command is found under the 3D Model tab, on the Surfaces panel.
To create the patch, select the three edges of the cutout and select "Apply". Repeat the process on the opposite side. You now have the cutout area completely surrounded with surfaces.
The next step is to create an Inventor Solid Body inside these surfaces using the "Sculpt" command which is located right below the "Patch" command shown above. Select the option to create a "New Solid" in the dialog box and then select the three surface features in the browser.
After selecting "OK" to finish, you will notice that a new Solid Body has been added to the model. Select it to confirm it is the triangular plug in the model.
The next step is to remove all the existing triangular cutouts from the original model, including the one used to make the new solid body. The Inventor tool used for this is the "Direct" command located on the 3D Model tab on the Modify panel.
Select the "Direct" function and select all the triangular cutouts in the model. You can use a "Window" selection method (left to right), maybe two, to make this job very quick. Select the "+" command to finish the task.
What you have left is the original solid body you imported and the triangular solid body that your created earlier. The next step it to remove the triangular solid body to create the triangular hole. The "Combine" tool, located on the 3D Model tab, Modify panel (see above) makes this an easy task. Select the original part as the "Base" and the triangular body as the "Toolbody" then "Cut" for the operation. Select "OK" to finish.
The last step is to pattern the feature (Combine1) to the count you desire. In my example, the array originally had 6 instances, I needed 12.
The process may seem long when you read and executed it for the first time but with practice, it will become a minute or two process. Also, think of the time you have saved not having to model the feature and possibly getting a dimension error or worse.
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