sheetmetal


Unit 5: Grade 10 Technological Design - Robotics - Sheetmetal Design

This unit will introduce you to SolidWorks sheet metal creation. This type of tool comes with several unique tools that work best with sheet metal designs. Creating sheet metal parts with SolidWorks is an important aspect of the program as this is a commonly used process in industry. Creating a sheet metal part can also be later flattened to see the pattern if the sheet metal part were all unbent and flattened out.

Course Units and Descriptions
Unit Description
Review course outline for more details
1 Careers & Safety- Intro, computers, organization, and careers
2 Technical Sketching- freehand sketching, ortho, dimensions, ISO views, custom ortho design
3 Basic 2D & 3D CAD Intro- 2D coordinates, lines, ortho views, 3D drawing, and custom design digitized
4 3D Parametric Design- 2D sketch, 3D parts, feature tools, drawings, exporting for 3D printing
5 Sheet metal Design- thin material design, folds, assemblies, 2D print, project design, testing, and build
6 Robot Assembly- part reproduction, part assemblies, custom function design and build
7 Web Portfolio- Showcase course work, projects, and understanding with web portfolio and presentation

Unit Content Activity Quick Links, Click to Jump to Specific Activity!

  1. Unit 5, Act. 1: Introduction to Sheet Metal in SolidWorks

- TOP - Unit 5, Act. 1: Introduction to Sheet Metal in SolidWorks

SW display

Situation:

Design and creating robots and similar mechanical components in Technological Design, sheet metal (SM) is commonly used. Using sheet metal to create bodies to support mechanisms is easier, lighter, and more efficient. For this reason 3D CAD programs need to be able to work with sheet metal in a virtual environment to create working designs that can be used for building and supporting mechanisms for the goal of the machine designed. Engineers use the Feature Sheet Metal tool set to create these designs using a set of related tools specifically designed to support the engineer to design and the manufacture to be able to build these machines made from sheet metal.


Problem/Challenge:

You are to explore the different methods of creating a sheet metal parts from a closed profile, open profile, and a solid material. Familiarizing yourself with the different tools through presentation and practice, then creating simple sheet metal parts, the 2 hole clip, a simple open box, and a final custom box with lid. Sheet metal parts will have drawings with orthographic views with proper placement of the front view, appropriate dimensions placed, isometric, and flat pattern shown. The final custom box will also be printed and built as a prototype.

Investigation/Ideas:

Investigation

A great introduction to sheet metal with SolidWorks should be reviewed. Being aware of the different characteristics of sheet metal, its manufacturing process, and advantages of using it, you will be able to design some effective and practical designs.

Sheet Metal in SolidWorks
sw-alignment

The Sheet Metal feature tools in SolidWorks, works with the basic characteristics of a thickness gauge of flat material with the ability to make and control bends. SolidWorks has built in gauge tables for thicknesses for different materials and your own custom tables can also be added. Bends tables are also provided to automatically calculate the standard bend radius and bend allowance based on material, thickness, bend radii, and bend angles, but custom bend tables can also be added.

When edges are bent, spacing and relief cuts with different shape options need to be considered. The spacing may be for clearance for the bend itself or you may want a gap for a weld to support and strengthen the design. A powerful option that SolidWorks offers, is to flatten your design so that the manufacture can cut out the pattern. Once the pattern is cut out, there may be additional holes, cut-outs, miters, and press forming prior to the bending, which may include simple straight bends, edge flanges, corner treatment, hems, rolls, lofts. The following are some common sheet metal feature tools that could be used with your design creation:

K-bending factor

  • Base Flange - creates sheet metal part from both open and closed sketches
  • Edge Flange - adds a flange that extends from existing model edge with alignment options Material Inside, Outside, and Bend Outside and relief cuts Tear, Rectangular, and Obround
  • Mitre Flange - similar to Edge Flange, but are made with a cross section open sketch and will automatically mitre corners
  • Hems - simple feature to strengthen edges created with a number of parameters in the property manager
  • Swept Flange - open profile perpendicular to a custom pathway of lines and/or arcs to create a sheet metal part
  • Forming Tool - is a mould to re-use through your SW Design Library to create unflattened features/shapes on your sheet metal part
  • Sketched Bends - allows you to draw a line on a flat closed profile and bend it on that line and should be careful with alignment options
  • Flatten - see your folded design in flattened state and be aware that flattened operations do not propagate back to the formed state
  • Unfold/Fold - if you need to complete edits or operations, use this tool rather than the flatten tool, so that
  • Rip & Insert Bends - starting with thin geometry based on extrudes and shells, you can manually convert to sheet metal with bend locations and rip or separation sections
  • Lofted Bends - using two open 2D open profiles, create a smooth transition from one shape to the other
SW-Command tool bar

Resources

The following support links are great resources on sheet metal (SM) tools and related information for use with SolidWorks (SW).

Links sw-sm-design

Create/Construct:

steps

For this activity you will create three major components: a simple bracket, a simple open box, and a custom closed box with a prototype build using different methods:

2 hole clip
Simple Bracket
Solidworks Drawing

Sample Model

Solidworks Drawing

Sample DWG

This will allow you to see two methods to build the same object, using first a closed 2D profile, and second by an open profile.

  1. Using the Simple Bracket tutorial steps, and/or video create the two hole clip using the imperial dimensions in the first tutorial, following their instructions and save in it's own folder tdj_2hole-clip-1_d-joe, file named: tdj_2hole-clip_1-d-joe.sldprt and tdj_2hole-clip-1m_d-joe.jpg
  2. Now create the same bracket, by making a 2D Sketch open profile using 12 gauge steel (gauge table) with a bend radius 0.13 inch with a K factor bend allowance of 0.5 then save in the same folder tdj_2hole-clip_d-joe, file named: tdj_2hole-clip-2_d-joe.sldprt and tdj_2hole-clip-2m_d-joe.jpg
  3. Using our custom template, make a drawing showing the three ortho views with dimensions, isometric, and the flattened view and save in the same folder tdj-2hole-clip_d-joe, file named: tdj_2hole-clip-2_d-joe.slddwg and tdj_2hole-clip-2d_d-joe.jpg
  4. Hand in whole folder for evaluation after you have completed and handed in the Solidworks Self/Peer Checklist sheet. Remember you must include 2 differntly created model builds, 1 drawing based on model 2 with jpg's (1 folder with 6 files)


simple box
Simple Box

Another simple sheet metal project, this time a box adding more tools to try out this time and building the model two different ways, to understand different build methods.

Some of the box specs are: 2 * 3", 1/16 thickness, relief circles 0.2", edge flange bends - outside blind of 0.75" with a bend radius about 0.075" and then a 0.15" open butt corner gap with a corner edge flange offset from surface also at 0.75" selecting offset from surface of 0.001" (sample flange settings).

  1. Following the steps in the Video Sheet Metal Box video, create the same box and save in it's own folder tdj_open-box_d-joe, file named: tdj_open-box-1_d-joe.sldprt and tdj_open-box-1-m_m-joe.jpg
  2. Next you will create the same box, this time starting with a solid 3D material, then use the convert to sheet metal tool to end up with the same box and will save in the same folder tdj_open-box_d-joe, file named: tdj_open-box-solid-2_d-joe.sldprt and tdj_open-box-solid_d-joe.jpg
  3. Using our custom template, make a drawing showing the three ortho views with dimensions, isometric, and the flattened view and save in the same folder tdj_open-box_d-joe, file named: tdj_open-box-2_d-joe.slddwg and tdj_open-box-2-d_d-joe.jpg
  4. Hand in whole folder for evaluation after you have completed and handed in the Solidworks Self/Peer Checklist sheet. Remember you must include 2 differntly created model builds, 1 drawing based on model 2 with jpg's (1 folder with 6 files)

box pattern
Custom Box Pattern and Build

This project, you will have the opportuntiy to decide on your box design and once your custom pattern is printed out in step 4, you will make it out of thin card stock to see if your design actually works.

  1. Review Video SolidWorks TNT - Design Cardboard Boxes with Sheet Metal Tips-N-Tricks video, note flange position is Material Outside, bend radius 0.001, and K factor to 0, then review Video SolidWorks Sheetmetal for Packaging example on making a basic box from scratch
  2. Create your own custom box with lid by either designing from scratch as above or by copying a picture pattern. The only restriction is, it must fit on a regular letter sized page at 1:1 scale if it were printed, so in other words, relatively small box
  3. Save in it's own folder tdj_closed-box_d-joe, file named: tdj_closed-box_d-joe.sldprt and tdj_closed-box-m_m-joe.jpg, then again using our custom template, make a drawing showing the three ortho views with dimensions, isometric, and the flattened view and save in the same folder tdj_closed-box_d-joe, file named: tdj_closed-box_d-joe.slddwg and tdj_closed-box-d_d-joe.jpg
  4. Also export a dwg file with geometry and bends only for print. Using the dwg file, open in Draftsight, add your name on the top centre of the box and print box pattern, cut out box pattern, and put together as a prototype.
  5. Hand completed files in folder and built prototype
challenge

Advanced challenge here is to download a vector pattern and export to .dxf file to import into SolidWorks and then resize if necessary to fit a standard letter sized page. Sample video showing part of this process called Video Folded Box in Sheet Metal, could be very helpful showing how to create a complex box pattern. Outside graphics could also be another option to add after pattern is complete. One place some patterns can be downloaded is from Freepik.


Evaluation:

evaluation

Ensure that you have included all required files and folders named in the correct naming conventions. Sample naming conventions have been provided above, which you could just copy and change the name. Remember your to dimensioning view placement, spacing, and scale properly.

Evaluation Breakdown Component Descriptions Marks
Always double check that you have completed all components for full marks.
Simple Bracket - two version model builds, ortho drawing, iso, flat and dimensions 15
Simple Box - two version model builds, ortho drawing, iso, flat and dimensions 15
Custom Box - closed box model, ortho drawing, iso, flat and dimensions, prototype 30