Create Custom Bill of Material Properties

When creating a Bill of Materials, it becomes apparent that different industries have different requirements; therefore there is a need to customize the bill of materials to present the required information.

Take for example the case of our simple part as shown below.

In order to customize the bill of materials we first need to create a custom property in the part.  To do this we go to File> Properties

In this example we are creating a property named Mass and it stores the weight of the part.  Under the Custom tab we enter our property name “Mass”, the type is text and the value can be selected from the drop-down menu, in this case we select mass and accept.

Our part is a component in the larger assembly as shown below

When creating a drawing for the assembly we want to go to Annotations> Tables > Bill of Materials and accept to create your bill of materials.

Once the bill of materials is selected you can right click the top of the bill of materials and choose to insert a column to the right to begin our BOM customization.

A new column is created and under property name we may select “Mass” which was previously defined in the part.

We now have a custom property in the Bill of Materials displaying the part mass.  This value will automatically update with any changes done to the part.

Changing Part Dimensions from Drawings

The process flow for SolidWorks usually starts with modeling a part / assembly and then afterwards creating a drawing from the model.  Usually changes are made to the model and they are reflected across all the drawings.  However it is possible to directly modify a part from the drawing. (Also Read: Drawing Zones in SolidWorks)

We have a simple part shown below (Related Read: Part Description Missing)

The part is detailed in the drawing shown below

In order to drive the dimensions in the model we go to the Annotations tab and select Model Items.

With Model Items selected, we want to select the drawing view and the dimensions to be driven as shown

Notice that the dimensions are black in color, not the usual grey.  By double clicking the black colored dimensions you’ll find you’re able to modify the dimensions. In this case we want to change the dimension to 200mm.

By accepting the changes, modification to the part is successfully applied to all drawing views.

Customizing Your Sheet Format

The sheet format forms the basis template for your drawings and customizing it to suit your needs is a fairly simple process.  In order to begin, open a new SolidWorks drawing and select the paper size as shown:

If your paper size is not listed or you would like to change the paper size of a pre-existing template, simply right click “Sheet1” > Properties and from that dialogue box you will be able to set your page size. 

Once you are satisfied with the sheet size, right click “Sheet Format1” and select “Edit Sheet Format”

When you are in “Edit Sheet Format” mode, you will be able to modify every part of the sheet template to suit your needs.  Editing a sheet is as simple as sketching in SolidWorks by using the sketch tools.  The icon on the top right hand corner serves as a reminder that the user is in “Edit Sheet Format” mode.  When the changes are complete click that icon and you will be ready to use your newly customized sheet format.

Weldments in SolidWorks

SolidWorks 3D CAD Design Software

SolidWorks Tutorial:Pi Day Candle Holder - DIY

SOLIDWORKS DIY (TUTORIAL): PI DAY CANDLE HOLDER

Pi Day is a celebration of the mathematical constant pi, 3.14159 or symbolized simply as π.  Pi  Day occurs on March 14^th and when written in MM, DD, YY format gives 03 14 15 or Pi!

What better way to celebrate Pi Day than to model your very own Pi Day candle holder.  This Pi day candle holder is designed to project the symbol π when lit. 

Let’s start with the solid modeling.  I have created my candle holder profile using a revolve function.  The profile is arbitrary.

Next, we apply a shell command.  In this case I have applied a shell of 3mm and have presented the results as a section view.

Orient yourself to the top plane and sketch the Pi symbol as shown. This will form the outline of the light projected from the candle.

Drawing the Pi symbol is not a trivial task, therefore we can place a picture of the Pi symbol onto the sketch plane for us to trace.  Access this tool by going to Tools> Sketch Tools > Sketch Pictures

Resize and trace the image as shown.  I have sketched the Pi symbol using lines and splines.

Create a reference axis from the center of the Pi symbol to the center of the flame by selecting two points.  Create one point on the Pi sketch and another point on a separate sketch approximating the center point of the flame.

Then use the extrude cut feature and be sure to cut along that reference axis to get your profile.

Use a circular pattern to repeat your cut as frequently as you like.  You are now done modeling!

Save your file as a STEP file.  This file can be used by commercial 3D Printers to print your part for you.  Consider printing ABS plastic so your product is more resistant to heat.

Congratulations you are now celebrating Pi Day in style!

Sketch Xpert in SolidWorks

Sketch Xpert

SolidWorks is a feature-based software and many of those features are created from sketches.  Sketches are composed of dimensions and relations to maintain geometry.  A blue sketch would indicate an undefined sketch whereas a black sketch would indicate fully defined sketch.  Image 1 is a good example of a fully defined sketch.

Sketch Xpert Image 1 (Defined Sketch):

There will be instances where a sketch will generate a conflict due to conflicting conditions. Also known as an over defined sketch.  In our case, Image 2 shows a tangent relation being added to a line and circular entity.

Sketch Xpert Image 2:

In cases like these we may use the Sketch Xpert tool.  The Sketch Xpert Tool is found from Tools > Sketch Tools > Sketch Xpert as per image 3.

Sketch Xpert Image 3:

Once Sketch Xpert is selected, click “Diagnose” and Sketch Xpert will search for a solution.

Sketch Xpert Image 4:

Under “Results” you may scroll through different solutions that Sketch Xpert has created in order to solve the conflicting over defined sketch.

Sketch Xpert Image:5

Sketch Xpert Image 6:

In this case we select the geometry that best represents what we wanted to achieve and select “Accept”. The sketch is no longer over defined and may be used normally.

Sketch Xpert Image 7: