Inventor Derive

Bob Wiley

1 Apr, 2020 09:01 PM

The derive command allows you to use models and assemblies as geometry and toolbodies within other part files. For 3D printing it's a perfect way to section complex parts so they can be printed in simpler pieces. Subsequent operations can be performed on the derived part without affecting the original source models and assemblies. Sketches, workplanes, and other work features may also be used from the source models.

1. Step 1: Create the derived part

   1. Open an existing part file or create a new one.
   2. Select "Derive"
   3. Select and open the source part or assembly file
   4. Select Geometry, Sketches and work features you would like to use. By default, visible features and sketches will be included. You may override these defaults.
   5. A scale factor may be applied. Also the source part or assembly can be mirrored.
   6. Don't forget to save your work early and often.
   7. The source model and any selected features and sketches are now available in the newly derived part. Unless brought in as independent solid body (more about that later), then all geometry of the source part is now a part of the derived part.
   8. Subsequent operations may be performed on this part without affecting the source part. If the source part is changed, then those changes will affect the derived part.
   9. The model is always brought in unrotated with it's origin at 0,0,0. You may move and rotate the source part after it is loaded. It is much easier if the original source model has an origin that allows subsequent use without requiring movement and rotation.
   10. Movement can be freeform or use relative coordinates. Assembly type constraints are not available. Movement can be cumbersome if complex placement is required. That's why it's recommended to have the model origin at a location that's ready for use.

2. Step 2: Perform operations

   1. Create work features and sketches like you would normally do. In this case I'm creating a sketch on the XY workplane
   2. Create sketch geometry. I highly recommend 100% constrained sketches. Be careful when placing constraints relative to source part geometry. It's often required. However, if the source geometry gets changed or deleted then it can break the constraints. That can be difficult to diagnose.
   3. Finish the sketch and perform extrude, sweep and loft operations as needed.
   4. Perform additional operations as needed.
   5. Don't forget to save your work
   6. This derived part can be modified in any way as if you were performing operations on the original source part itself. The modifications do not in any way effect the original part. Only the derived part.
   7. Multiple parts may be used as a source for the the derived part. They may be treated as independent solid bodies for subsequent join, cut, and intersect operations. Their geometry and features may be projected and used for any desired operations. If they remain independent solid bodies without subsequent join operations, they will be invisible not included in part geometry when placed in subsequent assemblies even though they may be visible in the derived part file.

3. Step 3: Use the derived part as a source

   1. Create a new part
   2. In this case I'm going to create a mirror image of the previously derived part.
   3. Here is the new mirror image of the previously derived part that includes all it's geometry.
   4. Save your work.

4. Step 4: Use the new derived parts

   1. Open an assembly
   2. Place the parts
   3. Constrain as desired
   4. Changes made to the original parts
   5. Are reflected in their derived parts
   6. Complex assemblies may be created using derived parts using a single source part. Changes to the source part are reflected in all subsequent derived parts.
   7. This avoids recreating the same geometry over and over for related parts and helps eliminate mistakes. Mirrored parts are truly just a mirror image rather than a complete remake of a part with details reversed.