Custom Drawing Template

A drawing template is one of the main components to any assembly or part drawing. A drawing template allows you to convey all information about a part or assembly in a clean and organized manner. The key features of a drawing template are simplicity and clarity. This blog will demonstrate how to make a simple custom drawing template in SolidWorks! 

Opening A Drawing Sheet

To create a custom drawing template, a blank template is needed to start the creation. SolidWorks offers multiple different sizes and shapes of pre-made drawing templates inside the programs files. One of these pre-made templates will be open and altered to make it blank.  Click on the new document command on the toolbar at the top of the screen or under the file drop-down menu. After trying to open a new file, a pop-up box will appear. Under the novice setting tab, there will be three options: start a part, assembly, or a drawing. Choose the create new drawing option. Another pop-up window will appear with a list of A-E drawing templates. These are SolidWorks default templates. Any size can be chosen but for this blog, the A(ANSI) Landscape template will be modified. An image of how to get to the custom SolidWorks templates is shown below in Figure 1.

 
 
 
 
 
 
 
 
 
 
 
 

Figure 1: SolidWorks custom template location

Clearing the Format

Once the pre-made template has been opened, the formatting needs to be cleared to be able to input a new custom template. In the feature manager on the left, there will be two features, these are “Annotations”, and “Sheet1”. Click the drop-down arrow next to sheet1 and another feature will appear called Sheet Format1. Right click on Sheet Format1 and select delete, the drawing template will then turn blank. An image of how to clear the format is shown in Figure 2.

Figure 2: Clearing the sheet format

Editing the new sheet

Now that the sheet has been cleared, a new format can be created on it. In the drawing, select the Sheet Format tab located on the toolbar near the top of the screen. Select the Edit Sheet Format command on this tool tab. After this command is selected the other two commands on this tab will become available to use. Now, select the Automatic Border command. Where to find these commands is shown in Figure 3.

Figure 3: Editing commands location

After the Automatic Border command is selected, the property manager will show a delete list selection box. Since the format is already cleared, this step is not needed. The blue arrow at the top right of the property manager can be clicked to move onto the next step in the command. After the blue arrow is clicked, the property manager will be filled with multiple different options on how to adjust the border that is being previewed on the drawing sheet. The zones, margins, line size, and borders can all be edited here. Once the desired sizes have been chosen, click the green check mark at the top of the property manager. There will now be a border around the drawing template. The Automatic Border property manager is shown in Figure 4.

Figure 4: Automatic Border property manager

Adding Sections

Now that the border is finished, some sections for information need to be added to help keep the template organized. To add in sections, they simply need to be sketched in. Go over to the sketch tab and select the line or rectangle command. Create some boxes and proportion them to the size and shape that is desired for the custom template. An example of the sections made for this blog is shown in Figure 5.

Figure 5: Example added sections

After the sections have been added in they need to be labeled. This can be done by placing annotations notes in each box. The Note command can be found under the annotation tab on the toolbar near the top of the screen. A note is placed in each box of the title block. This is done to give an input location for information about the drawing. Note size and shape can be adjusted by double-clicking on the note itself. An example of the layout for notes in a drawing template is shown in Figure 6 below.

Figure 6: Example section labels

Finishing Touches

Notice that there is still a large empty space inside title block area. Typically, in this space or one like it, a decal belonging to either the person or the company is placed to show ownership of the template. These pictures also help make the template look more aesthetically pleasing. For this blog example, the Perception Engineering logo will be added. To add a picture to the template the edit sheet format command must still be activated. If it is not, click on the command again. Go to tool on the toolbar at the very top of the screen and drop down the menu. Find the sketch tools menu and hit that drop-down menu as well. Under the sketch tools menu, there will be a sketch picture command. After clicking this command simply select the desired picture from its file locations and it will be placed onto the template. The picture can then be sized and edited in its property manager on the left-hand side. An example of this is shown in Figure 7.

Figure 7: Sketch picture example

Saving the New Template

Now that the new drawing template is complete, it must be saved! To save this as a template to be used all that is needed is to save the file as a drawing template (*.drwdot) file. After it has been saved as a drawing, the file locations need to be edited to pull the template. Click on the gear at the top of the screen and select file locations in the menu on the left side of the pop-up menu. Under the “show folder for” drop-down menu, select Document Templates. All that is left to do is select the folder that the drawing template was saved in and it can now be pulled to use as a template anytime! How to access the file locations is shown in Figure 8.

Figure 8: Editing the file locations

Final Thoughts

The purpose of a drawing template is to help with organization and presentation of a drawing and its information. A well-organized drawing template is a sure-fire way to portray professionalism when creating drawings. Even with just a simple template and title block such as the one shown in this blog, the look of a drawing can be increased as well as how easy it is to read and gather information.

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SolidWorks: Property Tab Builder

In this blog, we will be discussing the SolidWorks Property Tab Builder. The property tab builder allows the user to build preset properties that can be loaded into parts and assemblies. We will also look at how to integrate these into the SolidWorks Properties Tab, and some of the convenient ways to use the SolidWorks Properties Tab.

Property Tab Builder

To locate the Property Tab Builder, click on the Start Menu, scroll down until you find the folder called SolidWorks 2018 Tools, expand that folder and select the Property Tab Builder 2018.

 
 
 
 
 
 
 
 
 
 
 
 

Figure 1: Start Menu

Once the application is open, it should look like so:

Figure 2: Property Tab Builder

On the left-hand side of the window are the various elements that can be used to enter part property attributes. We break these down into further detail below. To add an element to the customer properties tab, click and drag the element into the Custom Properties column. Throughout this blog, we will be showing examples of how certain elements can be used in the workforce.

Groupbox

A groupbox is a feature that allows the user to group elements together within the Custom Properties and create sub-headings by dragging the elements into the desired groupbox area.

Figure 3: Groupbox

Textbox

The textbox field is used if you wish for the user to type in a value.

Figure 4: Textbox

The caption is what will appear as the title of the data entry box within the Customer Properties Tab. The name of the custom property attribute is what the inserted text will be assigned to within the part. The value is what the customer will be inputting when filling out the customer properties.

In this example, we will be using the textbox field to enter a part number the user wishes to assign to the part, as shown in the image below.

Figure 5: Textbox Information

List

The list element can be used to create a drop-down list for the user to select from a variety of values.

Figure 6: List

One example of how to use the list element is by having the user select what category the component can fall under. In this case, the user has the option to select Manufactured, Purchased, or Fastener.

Figure 7: List Properties

Number

A number element is a useful tool for a user to increase or decrease a numerical counter for the desired attribute.

Figure 8: Number

One example of using the number element is by creating a counter for the desired quantity of a part to be manufactured, whether there are more than one in an assembly or a replacement part is desired. The image below shows the use of using the number element for BOM quantities.

Figure 9: Number Properties

Checkbox

Another custom property element that can be used is the checkbox.

Figure 10: Checkbox

An example of the checkbox is using it as a Yes or No indicator. In this case, we are using it as an indicator for the user to identify whether the component is constructed out of sheet metal or not.

Figure 11: Checkbox Properties

Radio Button

The radio button element is very similar to that of the checkbox, but it can allow the user to select from a variety of variables.

Figure 12: Radio Button

A popular practice in the sheet metal industry is to indicate the surface class of a part. We used different surface classes as the variables for the radio button element as shown below.

Figure 13: Radio Button Properties

Once all the elements and attributes you wish to include have been added to the custom properties, save the file to your desired location. You can save the file as a part, assembly, drawing, or weldment custom property file by changing the type under the Control Attributes column.

Figure 14: Property Types

SolidWorks Property Tab

If you open a new part using the templates provided by SolidWorks, the part properties should be blank like so:

Figure 15: Blank Part Properties

Now go through and link the file location of the custom property files to the location where you save the custom part property file. Once that is completed, go to the Custom Properties Tab on the right-hand side of the screen. You should see the part properties we created in the property tab builder.

Figure 16: Custom Properties Tab

Now fill out the elements within the tab as shown below and click apply.

Figure 17: Custom Properties Tab Information

If we go back to our part properties, they should include all the information we added to the custom properties tab.

Figure 18: Part Properties Populated

The custom property files are a great tool for implementing part properties into STEP files that you have downloaded, or even for updating the properties of a file that might be out of date. This is a more efficient method than copying part properties from one file to another.

That’s all for now! You now know the basics to create a custom property file. If you like the content or have questions, signup for our email list to stay in the loop for solutions or weekly content. Cheers!

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Part Configurations

Often customers will want to view multiple configurations of the same part to see which they like best. Instead of creating four or five new part files to show the customer, it is much easier to create each version of the same part with the configurations manager tab.

Configurations

Within the configurations tab on the feature manager tree, right click on the Part and select Add Configuration.

 
 
 
 
 
 
 
 
 
 
 
 

Figure 1: Configuration tab location

Organize Configurations

Each configuration should have its own unique name to quickly distinguish between each configuration. This will help distinguish each configuration within assemblies and drawings to ensure the correct model is chosen.

Figure 2: Configuration Name

The saved configurations will appear in a pop-down menu within assemblies and drawings as seen below. Simply click on the part and the option to choose between each configuration will appear. Keeping simple and descriptive names will be the best option for configuration models.

Figure 3: Pop-down Menu

Modifications to Configurations

The feature tree model gives the option to suppress and unsuppressed features. Each configuration will be slightly different which means some features will need to be suppressed and others unsuppressed depending on the design intent. The default configuration should be the original design before modifications are incorporated.

Default:

Figure 4: Default Bracket

Large Mount:

Figure 5: Large Bracket

Small Mount:

Figure 6: Small Bracket

The reason each configuration has its own hole wizard feature is to ensure it has no relation to any other configurations. If bracket were to have only one clearance hole, then all three configurations will be identical; hence the need for three separate hole clearances.

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Pattern commands are a designer’s best friend in terms of replication and improving overall efficiency. Linear, Circular, and Curve driven patterns are all common commands used by the everyday CAD user. This blog will guide you through using these three pattern features in SolidWorks and provide context as to when they can be used to simplify the modeling process.

Linear Driven Pattern

The Linear Pattern Command is used to drive features, faces, or bodies in a linear direction.  This feature helps save time by cutting down the repetitive movements of adding a bunch of holes or other forms of geometry. In Figure 1, the location of the linear pattern command in addition to the curve and circular driven pattern commands are shown.

 
 
 
 
 
 
 
 
 
 
 
 

Figure 1: Command Locations

Using an existing hole wizard feature, the linear pattern will systematically generate identical holes across the model. The first step in executing a linear pattern is to select a desired feature in the Features and Faces selection box or by preselecting prior to hitting the Linear Pattern Command (Figure 2).

Figure 2: Selecting the Feature

After selecting “3/4-10 Tapped Hole1” feature in this case, the dimensions defined in the feature appear and can be used to aid in the patterning process (Figure 3). The next step in the command manager is selecting up to two linear pattern directions. For this example, the two 4.00 dimensions were used to define two pattern directions, as they are in the desired linear direction to make an equally spaced square hole pattern. Additionally, there is also the option to select edges, faces, planes, and other geometry in the preferred linear direction.

Figure 3: Setting Direction

Now that the directions are set, the next step is to fill out the necessary parameters for each direction required to make the pattern. The first parameter is the number of instances. As seen in Figure 4, the desired “3/4-10 Tapped Hole1” hole feature pattern will add 2 instances in both directions creating a 2×2 square. The distance in both the vertical and horizontal direction was set to 12 inches in order to keep the pattern centered to the square piece.

Figure 4: Hole Instances

If the desired pattern direction is oriented incorrectly, the opposing arrows button (highlighted) next to the selection box flips the direction relative to the reference selected. Figure 4 also shows a pattern preview on the part (enabled from the checkbox on the bottom of the command manager), which will help verify the orientation and intended pattern direction.

Lastly, as seen in Figure 5 the green check mark in the top left corner of the manager will execute the command and reveal the pattern on the model.

Figure 5: Final Check

Curve Driven Pattern

In the next example, the Curved Pattern Command is used to execute a hole pattern consistently about the outer curvature of a cam (see Figure 6). The setup and command manager layout are nearly identical to the linear pattern and the steps are listed below as follows:

– Select the feature/face/body to pattern

– Select a curved reference (this can be an open or closed curved geometry)

-Adjust the direction, spacing, and number of instances in the desired pattern

-Preview the pattern and then execute.

In this curve driven pattern example (see Figure 6), I selected a hole feature, the edge of the cam as the Direction 1 reference and adjusted my instances and spacing to 4 and 0.425 correspondingly. As with the linear pattern, up to two different directions can be added.

Figure 6: Curved Pattern About an Edge  

Circular Driven Pattern

The Circular Pattern Command is an excellent tool used to replicate features, faces, or bodies in a rotational manner about an axis. In this example (see Figure 7), I show how to replicate an extruded cut with filleted corners about a round piece of tubing.

Figure 7: Circular Pattern Overview

Similar to the linear and curve driven pattern, the first step is selecting a feature (or features in this case) to replicate in the Features and Faces selection box or by preselecting prior to hitting the pattern command.

Figure 8: Selecting Features and Faces

After the cut-extrude and fillet are both selected, the intended rotation axis is selected in the top selection box under Direction 1 in the command manager (see Figure 9). The rotation direction can be toggled using the arrow button to the left of the selection box. The next step is to select the degree of spacing and number of instances.

Figure 9: Circular Pattern Parameters & Preview

In this example, since the original extruded cut through both sides of the pipe, the pattern only needed to rotate the feature 180 degrees instead of 360 to complete the cut all the way around, so I chose a 45-degree spacing and 4 instances to complete the pattern across the tube. As with other pattern features discussed, up to two directions can be selected.

That’s all for now! You now know the basics in Linear, Curved, and Circular Patterns. If you like the content or have questions, signup for our email list to stay in the loop for solutions or weekly content.

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Feature Mirroring

While creating parts in SolidWorks, efficiency and accuracy are essential when working on a project for a client! For projects that are repeatable, Perception Engineering saves time by applying the mirror feature command if models are symmetrical. SolidWorks is equipped with a few different types of mirroring commands: sketch mirroring, part mirroring, and feature mirroring. For this blog the focus will be on feature mirroring utilizing the given top, right, and front planes to create feature mirrors!

Getting started

The mirror icon is located on the feature command bar as seen in Figure 1.

 
 
 
 
 
 
 
 
 
 
 
 

Figure 1: Mirror Icon

To ensure proper use of this feature, be sure an extrusion is modeled. This feature will mirror the extrusion over a desired plane. A simple exercise to do is to create a feature on the front plane and have it share one edge with the right plane as shown in Figure 2. This feature works the same no matter how complex the model, as long as it has one shared edge with a plane.

Figure 2: Highlighted shared the edge with a plane

Plane and Feature Selection

Now that you have a feature ready to be mirrored, such as an extrusion. Select the mirror icon on the features toolbar. The first selection box asks you to pick a mirror face/plane. Select the right plane as the mirror plane, then the right plane will appear in the selection box, as seen in Figure 3. Now, all that needs to be done is select the feature that is to be mirrored. The second selection box asks for a selection of a feature to be mirrored. It is possible to click directly on the feature itself to select it, or it can be selected on the feature manager tree. Once the feature that is desired to be mirrored is selected it will appear in the selection box.

Figure 3: Property manager

There is also an option to choose a 2D face to mirror instead of a 3D feature. By using this option, you cannot mirror bodies but only surface face features such as holes, surface cuts, and other features that are placed on an already created 3D body. To do this correctly, the face must be mirrored onto an already created feature, the face cannot be mirrored into blank space to become its own feature.

Figure 4: Faces to Mirror

The ability to mirror faces can be very helpful. If there are multiple complicated features on an extrusion body, rather than draw out every one they can simply be mirrored to the desired locations.                                                                                                       

Preview Selection

There is an option to preview the mirror at the bottom of the property manager, as seen in Figure 5. If the partial preview is selected a 2D highlighted copy of the newly mirrored feature will show across the right plane from the original feature. If the full preview is selected it will highlight both features showing that the outcome will be one combined body with an extrusion depth shown in 3D. All there is left to do now is click the green check at the top of the property manager and mirror the feature!

Figure 5: Preview modes

Reasons to Mirror

Mirroring is a simple and easy way to save time when modeling parts. Mirroring is used primarily to create perfect symmetry for a part, this way you only need to make half of the part in only half the time! Mirroring can also be used on more than just part bodies, it can be used on smaller extruded features, cuts, and various shapes that appear symmetrically throughout the part.

Figure 6: Fully Mirrored

The team here at Perception Engineering use the mirror command to save time when the part model is similar in geometry. Both features and sketches are used in the modeling phase regularly so having the models orientated symmetric along the top, right, and the front plane will save some time.  

Thanks for tuning in our weekly blog! Please subscribe to our weekly postings and feel free to ask us any questions or concerns and our team will get back to you. 

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Exploding an assembly view in SolidWorks can make all the difference when trying to show every component involved in the making. Instead of showing multiple views and angles, one view can be used to show all components. A well done exploded view will also help in the understanding of how the entire assembly fits together. Exploded views are used in almost every industry when it comes to explaining a product and how it works. Knowing how to use the exploded view feature is a crucial key feature and will be finishing touch needed when showing an assembly.  

Feature/Icon Location

Exploded views are only able to be performed on an assembly, not a single part. Therefore, the exploded view icon is only located inside of an assembly file. To reach the icon it can either be found on the assembly tab toolbar or can be created by going under the configurations tab and right clicking on the assembly icon and creating a new exploded view. Both locations are shown below in Figure 1.

 
 
 
 
 
 
 
 
 
 
 
 

Figure 1: Feature/Icon locations

Exploded View Feature Manager

There are two types of exploded view step types to choose from, as seen in Figure 2. There is a regular step and radial step. By choosing regular step, objects selected, being one or multiple, will all move in the same direction with each other. The radial step type is mostly used on parts that are in a circular type pattern. When using a radial step, all parts chosen will move away from each other from a common center point when dragged. Almost as if they are lying on a circle that’s radius is expanding. The focus of this blog will stay on regular step exploding since this is the most common type to be used.

Figure 2: Explode step types

Exploded part selection

Exploding an assembly using regular step type is quite simple. After choosing the step type the components that are desired to be moved are selected and dragged, this can be one part or multiple. If multiple parts are highlighted at the same time they will all move in the same direction when pulled. The direction is chosen by the user. After clicking on a part to be moved an origin point is shown on the selected part showing the possible direction and rotation options. Simply click and hold on the arrow in the direction that is desired and drag the mouse. After the components are moved an “exploded step 1” will appear in the exploded steps view box inside the feature manager. From here previous steps can be edited by right-clicking on them. An example of these steps is shown in Figure 3 below.

Figure 3: Explode step 1

Under the part selection box in the feature manager, there is the option to input set values for how far the part will move and what rotation angle can be put on the selected part. These can be used for exact spacing of exploded parts if it is needed. There is also an explode direction selection box located below the part selection box, as shown in Figure 4. In this selection box, the direction of the exploded step can be changed to match a face or axial direction of another part located inside of the assembly. This can help in the overall flow of the exploded view, giving it a cleanly spaced look when the exploded view is finished.  

Figure 4: Set value locations & Explode direction change

Other Exploded Options

Located at the bottom of the exploded view feature manager are a few other options to choose from when exploding an assembly. A very helpful one is the option to turn off and on select subassembly parts. This allows you to move a subassembly as one whole part or one part of the subassembly at a time. This option can only be applied if there is a subassembly inside the assembly that is being exploded. There is also a button that gives the option to reuse a subassembly explosion. If a subassembly being used has already previously been exploded, by clicking this button that exploded state will be shown and it will not have to be redone! These options are shown in Figure 5.

Figure 5: Subassembly explode options

After Exploding The Assembly

Once the assembly has been fully exploded it can be quite hard to tell just exactly where everything has come from and where everything goes back to. Especially in an assembly with a large number of parts. There is an option to add smart explode lines to help with this. These lines, when added in, follow the path that every part was dragged from all the way back to its origin. This helps greatly in showing how an assembly is put together. However, if there are a large number of parts the lines can become cluttered and overwhelming, this option can be left up to personal preference. In Figure 6 below a final exploded assembly is shown with smart lines as well as the location of where to add in the smart lines. 

Figure 6: Full exploded view with smart lines

Things to look out for

When exploding an assembly, make sure all components can be seen from one view. Typically for exploded assemblies, the viewpoint is from an isometric view. Also, when exploding an assembly, after clicking off a part, the assembly may collapse and go back to its original state. You do not have to redo the entire exploded assembly. Simply go back to the configurations tab and under the exploded view configuration, right click and hit edit feature, the assembly will re-explode.

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This blog will show three basic examples of how to use the Swept Boss/Base feature in SolidWorks. There are two main requirements to create a Swept Boss or Base: A closed profile and a path. This first example will show how to create a sweep using a circular profile and an open relatively linear path. Figure 1, below, shows the profile drawn on the front plane and the sweep path drawn on the top plane. It is important to make sure that the starting point of the path lies on the same plane as the profile. Also, notice how the center of the circle profile is centered on the start of my path. This ensures that the sweep will be centered to my profile; however, any location contained inside the profile, including the boundary, can be used to generate a sweep.

 
 
 
 
 
 
 
 
 
 
 
 

Figure 1: Profile and Path

Once your profile and sketch are defined, select the Swept Boss/Base command on the features tab as seen in Figure 2.

Figure 2: Swept Boss/Base Command

The command window will then appear on the left side of the screen. Click on the boxes under the Profile and Path section and select your profile and path sketches as seen in Figure 3. A preview of your sweep will appear to further verify your intended feature.

Figure 3: Command Manager & Execution

The green check mark on the top left of the command manager will execute the command and reveal the finished model as seen in Figure 4.

Figure 4: Example 1 Finished Model

This first example shows the basics of generating a sweep feature. Examples 2 and 3 dive into more complex geometry and some other capabilities of this command. Figure 5 shows the cross profile and the slot-shaped path used for the sweep in Example 2.

Figure 5: Example 2 Profile and Path

Selecting the Swept Boss/Base command and the two sketches above as the profile and path accordingly, Figure 6 shows the initial preview of the sweep. Expanding the options drop down in the command manager, as indicated by the red arrow in Figure 6, SolidWorks allows you to change the orientation of the profile along the sweep by assigning a profile twist. The profile twist can be specified by a twist value, direction vector, or by applying tangency to adjacent faces. In this example, a profile twist value of 720 degrees (also available in radians or revolutions) was set and can be seen in Figure 7.

Figure 6: Example 2 Command Manager and Preview

Figure 7: Assigning a Profile Twist

After hitting the green check, the resulting model from the sweep feature is shown in Figure 8.

Figure 8: Example 3 Model

This final example will cover how to setup and execute a sweep using guide curves. Guide curves in comparison to profile twist allow for a varying profile size along the path of the sweep. Figure 9 shows separate sketches of the square profile, line path, and the additional guide curve drawn on the same plane as the path. Make sure when adding a guide curve to a sweep that the pierce constraint is used to connect the start of the curve to the edge of the profile (see Figure 9). In utilizing guide curves, it is also crucial that profile of the sweep is not fully constrained otherwise the sweep will fail. In this example, the height of square profile is constrained but not the width.

Figure 9: Adding a Guide Curve Sketch

After sketching the profile, path, and guide curve on separate sketches, enter the Swept Boss/Base command manager and add in the profile and path designated in Figure 9 above. Select the guide curve drop down and, in the box, select the guide curve sketch from the feature tree (see Figure 10).  Since the width of the profile is not constrained, it can follow the guide curve as it is swept down the intended path. After executing the command, the resulting model is seen in Figure 11.

Figure 10: Adding a Guide Curve in the Command Manager

Figure 11: Example 3 Model

That’s all for now! You now know the basics of the Swept Boss/Base. If you like the content or have questions, signup for our email list to stay in the loop for solutions or weekly content.

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