This year there are a number of new features in Inventor based around mesh manipulation and the shape generator. Taking an overall look at these features we can see that they are all centered around enhancing Inventor’s abilities with generative design and handling mesh outputs from simulation environments. There are a number of reasons why you might end up needing to work with a 3D mesh model in Inventor though.
Here is a mesh model I downloaded from instructables.com for making your own 3D printed quadcopter. The design is fairly simple and serves its purpose well but what if we wanted to make some changes to the design?
As of Inventor 2016 there was not much you could do with meshes directly. However, in Inventor 2017 the ability to work with meshes has been addressed and a number of tools come together that allow more than a straight mesh import.
The CAD files included with this instructable are STL files intended for 3D printing, not modification. The top and bottom of the quadcopter and the prop arms. Well, if we want to modify the design we will need use the STL mesh files to create a 3D parametric model. I am working with the top portion of the enclosure here.
Taking advantage of Inventor’s AnyCAD tools we can open the mesh directly as a part file or import the mesh after creating a new part. Either way once you have the mesh in Inventor’s part environment it’s time to start building new features by reusing the mesh geometry. The key is the new Fit Mesh Face command in the Surface panel.
Using the Fit Mesh Face tool we can select facets on the mesh and have Inventor create surface geometry of different shapes that are coincident with mesh vertices. There are options for creating planar surfaces, cylindrical, spherical, toroidal and complex surfaces, plus an auto option which will determine which of the face types your selection best fits.
Note: For complex shapes you could use a combination of this tool and existing Inventor surface tools to come up with a volume that can be stitched together and converted to a solid.
The brush size here controls the selection picker diameter for selecting mesh facets. This size is tied to screen dimensions and not the zoom or absolute size of your model. As you zoom in and out there is no change in the selector diameter but more or less of your model will fit inside based on its zoom position.
By selecting some facets on the bottom surface of the mesh and clicking OK I have created a planar surface. The Auto Fit option could see that my mesh selections were all planar.
With this face created, even though Inventor sees the result as a surface feature in the model browser, we can use it as a sketch face since it is planar (you could also select the bottom of the mesh object directly if it is planar for use as a sketch plane). Once in the sketch environment we can use new Project Geometry selections to pick edges from the mesh and project them into our sketch. Most often mesh edges can be selected directly but occasionally Select Other needs to be used. Depending on the operation Mesh Edges, Mesh Faces or Mesh Vertex selections can be made.
Now, we can continue building our model using standard feature tools. Since I am extruding the overall depth of the quadcopter body I want the extrusion depth to be the same as the existing mesh. Unfortunately using the To option in the extents area of the extrude dialog box is not possible since facets & edges cannot be selected here. Instead, I can use the measure tool and measure the distance between parallel mesh facets or vertices. I could also measure the length of mesh edges.
With a base feature in place making a solid body I can continue modelling. I created a second sketch on the bottom of the part for all the cutouts and projected the mesh edges, shared the sketch and made separate cut features for each cutout. From this point I am free to modify the design as desired. I could also have used the projected lines as construction geometry and designed around them in the sketch.
Since this will be printed in ABS the material has been changed in Inventor also. What’s left is to create the bottom and the prop arms in Inventor and add the electronic components in the design. I will address some different ways we can manipulate these parts in upcoming posts.
-DP
