Ask and answer engineering questions

Learn from millions of experts

Feed

Drive Sheet metal parts from a layout sketch

By lawrie on 28 Jul 09:33 1 answer 531 views 0 comments

Example of a fan scroll sheet metal part that uses a layout sketch, parameter file and design function / equation table.

Geomagic Design added a global parameter function in the latest release. ver. 17, from main window, File -> New-> Global Parameters to create a new file ( Capture 1 ) and create a new parameter, ROTOR_DIA with a value of 400mm ( Capture 2 )

Start a new sheet metal part and select a plane to make the layout sketch ( Capture 3 )

Open function editor and attach the global parameter file you created (Capture 4 & 5 )

The layout sketch ( Capture 6 ) is created. The circle, centered about origin, corresponds to the fan's rotor dia. The set out square. also centered about origin. gives 4 points to strike the 4 arcs that will form scroll. Fully dimension this sketch and using function editor the dimensions that drive sketch are linked with equations that are functions of the global parameter ROTOR_DIA ( Capture 6a ) e.g the circle, ROTOR = ROTOR_DIA = 400 RAD_1 = ROTOR_DIA * 0.7 = 280. Due to having this sketch fully restrained, RAD_2, RAD_3, RAD_4 and ANG_1, ANG_2, ANG_3 are driven dimensions and ANG_4 is given, in this case a value of 30 deg. These dims are labeled as they will be used to create sheet metal.

Plane 1 is offset from YZ plane by a distance equal to RAD_1 + (SQ/2), on this plane sketch 2 is placed, a rectangle that will be used to generate a sheet metal face that is the base feature of this part ( Capture 7 ). The dims of this rectangle are generated as functions of ROTOR_DIA, height, ROTOR_DIA * 0.65, width, ROTOR_DIA * 0.25, Top, from origin, height + (SQ/2).

The sheet metal properties are configure to suit (Capture 8 ) ( Capture 9).

The Flange tool is used to create the 4 arcs that form the scroll ( Capture 10 to 13 ). Note that the bend only option is selected, the inside edge is chosen and bend angle and bend radius are selected in sequence from Rad_1 to RAD_4 and angle ANG_1 to ANG_4. The finished part should be like Capture 14. The result is a fully functioning sheet metal part that can be flattened ( Capture 15 ).

The big advantage with this approach is that you end up with part that can be easily be re-used and adapted for a complete range of fans. A range of fans will be, for each particular type, geometrically similar, with rotor dia, and motor size to suit required volume of air at required pressure determined by rotor dia and rotor speed. All parts can be driven by a single linked global parameter file ( or linked spreadsheet ). Change variables in this file and you can generate complete manufacturing drawings for complete range easily and quickly ( Capture 16 & 17).

Although, for this example, I have been using Geomagic Design, I have also done somewhat similar things with Solid Edge and Solid Works, same approach but as each software works slightly differently not quite the same, should be same with Inventor. Compared with the tools available when I started in this profession 3D CAD modeling adds many advantages to the whole design and build process, way faster than the old way with hand drawn designs.

1 answer

Add your answer to: "Drive Sheet metal parts from a layout sketch "

Save Cancel