Objectives Inventor Part Modeling MA 23-1 Presented by Tom Short, P.E. Munro & Associates, Inc To demonstrate most of the sketch tools and part features in : Inventor Release 6 And, to show logical techniques and guiding principles that create robust, elegant, and parametric parts. Troy, Michigan 48084
Setup of screen Origin point, axis, and planes Construction style Dimensions & Edit now Extrusion Constraints Materials 1. Construct accurately when possible 2. Use construction geometry and constraints 3. Create fully constrained parts 4. Keep the first sketch simple Example 1A Dimension Construction Circle Normal Rectangle Fixed Point Constraints Common View Multiple windows New Sketch Project Geometry Hole Point Holes Threads Mass Properties 1. Use existing geometry when possible Example 1B Multiple Views Threads Displayed Common View Right Mouse Edit Select
Example 1C Example 1D Work planes and axis Project Geometry Extend and Trim Revolve Equal Constraint Project Point Circle & Line Creating Work Planes Project Geometry Holes to a face Revolve Equal Constraint Help on work planes Pick Here then Here Selecting a profile Selecting a profile Extrude Cut All Mid-plane Extrude Cut All Mid-plane Mass Properties Colors 3 Lines Project 1. LEARN all work plane choices! Equal Constraint
Example 1E Example 2 Rectangle Fillets, edges and loops Colors Textures Text & Emboss 1. Put fillets and chamfers on close to last Fillet edges of rod first then you can select loop at intersection Precise Input Relating dimensions Parameters 1. Relate dimensions where possible for parts that need to change Apply Texture Add the vertical dimension relating the two Construct a rectangle from 0, 0 to 5, 4 and dimension the base This is d0 Or create user parameters relating the dimensions Apply Texture
More Parameters Trim Mirror sketch Circular Pattern 1. Build parts that are parametric Example 3 Spur Gear Sketch a circle with a diameter equal to the root diameter and extrude it 1 back Units are important and you may have to correct an equation to get them right! Example 3 Spur Gear Con t On a new sketch draw a vertical construction line from the center Draw a line from the center and dimension the angle to (360 deg / NT / 4)*1 deg this is 5.00 degrees Dimension the length to PD/2 the end of this line is the pitch point Draw a line thru the pitch point and dimension it to 75.5 degrees Draw a line perpendicular to the previous line At the end of this line, construct a Normal circle thru the pitch point Mirror the circle about the vertical centerline. Then trim both circles to arcs Extrude this shape to the back face of the gear. Fillet the root intersections at a radius of 0.2/DP Create a circular pattern with NT items in 360 degrees. Pick the tooth & the fillets as features.
Example 3 Spur Gear Con t Create a new sketch on the visible work plane. Don t place it on the face of the gear! Draw two concentric circles Dimension the inner one with a diameter equal to OD the outside diameter Dimension the outer one to OD + 4*AD Extrude the profile of the annulus, cut, thru all to cut off the tops of the teeth. Note the size of the file. (289 kb) Change the number of teeth in the parameters and update the gear Sweeps Example 4 Sweeps Sweeps require that you have 2 unconsumed sketches. The profile and the path.
Example 4A Helical Gear Start with the same tooth profile Create a work plane at the helix angle to the Y-Axis Use the new plane as a Split Tool to split the face of the cylinder generating a helix path Make a new sketch on the new plane and project the helix path Sweep the tooth profile along the path Plane at helix angle Loft Mirror part Shell Loft requires 2 or more sketches on various planes. The transition at the first and last sketch can be controlled by the Conditions tab. Mirror requires one or more features and a mirror plane. Shell requires removing faces that are open. Example 5 Lofts Fillet the tooth, make a pattern, trim off tip, and clean off back