Amazon Part Finder

Do you have a random screw, washer, or nut laying around and have no idea how to identify what it is? You’re in luck with Amazon’s new Part Finder option within the Amazon app! Amazon now has the technology to scan whichever type of desired fastener, provide accurate sizing of it, and provide links on their app so you can purchase these! This blog will highlight how to locate this function within the app and how to use it.

Locating Part Finder

Locating the app is actually easier than what some people may believe because it is actually located in the regular Amazon app. First, download the Amazon app from the iOS App Store or the Google Play store for Android. Once the app is downloaded, select the camera next to the search bar to access the Part Finder function and many other useful options. Access to the camera will also need to be allowed to use these options.

Figure 1: Camera Location

Once you’ve selected the camera option and have allowed access, Amazon’s default function that appears in the Product Search option. To locate Part Finder, select the see more option at the bottom of the screen and select the icon of a screw with the Part Finder text below it.

Figure 2: Locating Part Finder Option

How to use it

Now that the Part Finder option has been located, the next step is to try it out! Along with the app, there are a couple of things that will be needed. You will need a fastener, washer, or nut to be measured, a white surface (a piece of white paper will work), and a penny. The white surface helps the camera get a clear picture or the threads and the penny is for reference to get an accurate size of the object. Once those are located, take a single object, we’re using a bolt for example, and place it next to the penny on the white surface.

Figure 3: Example Bolt with Penny

The next step, with both the penny and object being measured in the frame, hold the phone level and steady. If you’re unsure if the phone is level, try and match the white circle into the center of the intersecting lines (the lines will turn green and the countdown will begin once the phone is level).

Figure 4: Measuring the Object

The app will now start to analyze the photo and once that’s complete, it will prompt the user for some extra inputs. The user will need to select a few options: which type of screw it is, the head style, and the drive type.

Figure 5: Scanned Photo and Extra Inputs

After the parameters have been set, select the See Search Results on the page in the bottom-right corner and Amazon will open what they believe to be the correct screw within the app. Depending on how the photo was analyzed, Amazon will provide the length and the diameter of the object (different items appear at the top from when measuring a nut, washer, or bolt). The app will also provide links to the measured objects that can be purchased directly from Amazon.

Figure 6: End Result

Conclusion

Even though this technology is still fairly new, it’s improving and only becoming more useful and smarter with each released update. The only complaint with this current version is that it can’t identify threads which would be very useful. Maybe in future updates, we can have this option along with other quality of life updates!

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SolidWorks: Linear, Circular, and Curve Driven Pattern Commands

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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SolidWorks: Feature Mirroring

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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SolidWorks: Introduction to PDM

SolidWorks Product Data Management (PDM)

Team Collaboration, you may love it, you may hate it, but it is often necessary when it comes to coordinating projects among teams. There are many tools and applications designed to go about streamlining this process, however, there are better choices for specific purposes. Here at Perception Engineering much of our work is design work done through SolidWorks. To make our team project collaboration more efficient we have implemented SolidWorks PDM. This blog will go over what that is, some of the functions we have found particularly useful, and how to set up your first vault.

Introduction to SolidWorks PDM

SolidWorks PDM stands for SolidWorks Product Data Management. It is an add-on package that provides you with the tools to manage and coordinate your files while being very closely integrated with SolidWorks. It allows you to create file vaults within your computer’s file explorer that allows each team member, that is appointed access, to check files in and out of on their own computers. Once a vault is created, files can be uploaded and organized into folders within the vault. This program is especially useful for SolidWorks. Team members can check out design files, make their changes, and check them back in. This allows for collaboration on a part without working on the same computer. There are also features such as folder and file data cards which allow you to change your part properties from the file browser; also making it possible to change multiple parts’ properties at once. You can also create workflows to streamline the approval process of a project. With these, you can designate team leaders to oversee the status of a document submitted for approval which will automatically update revisions of a SolidWorks file. More in-depth walkthroughs of these features will be included in future blogs.

Starting a New SolidWorks PDM Vault

The first step to creating a vault within PDM is to open the Administration application, which will most likely be found in your programs file on your computer.

Figure 1: Administration Application Icon

Next, you must add the server that your team plans to work on. This can be done by selecting “File” → “Add Server” and following the prompts. Once this is complete you are ready to add your first vault. To do this you must use the drop-down menu for “SOLIDWORKS PDM Administration” and right click on the option that has your server name and select “Create new vault…”.

Figure 2: Location of Vault Creation

This selection will bring you to the “Create New Vault” wizard. This will walk you through the rest of the steps needed such as selecting the type of vault, naming your vault, and where to place it. Once you reach the “Choose database” page, if your server is not an option on the drop-down menu make sure to type in your server name in the edit box provided.

Figure 3: Database Entry in Vault Wizard

You will then continue through the wizard, choosing the settings that you prefer. Once you reach the “Configure vault” page, it is suggested that you use the predefined configuration, “SOLIDWORKS Quick Start”. Carry out the last few pages of the wizard, select finish and there you have it! Your first SolidWorks PDM vault.

That’s all for now! You now know how to set up your own SolidWorks PDM file vault. If you like the content or have questions, sign up for our email list to stay in the loop for solutions or weekly content.

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SolidWorks: Exploded Views

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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SolidWorks: Swept Boss/Base Command

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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SolidWorks: Online Licensing Troubleshooting

Troubleshooting SolidWorks Online Licensing

New to SolidWorks 2018, Online Licensing offers users the flexibility of accessing SolidWorks licenses through online MySolidWorks profiles. An administrative portal on MySolidWorks gives designated users the ability to assign seats of SolidWorks to members of their team. While this option is a huge step forward, in comparison to machine activation/deactivation using the modify install, implementation of online licensing companywide has uncovered many issues that have yet to be solved by SolidWorks upon their first release. This blog will hopefully ease a headache when running into errors, while trying to convert workstations over to online licensing for daily use. For help with using the administrative portal, switching serial numbers to online licensing, and for general procedural directions using online profiles in SolidWorks please reference the link at the end of this blog.

Activation issues

After following the procedure to make the switch from machine to online activation in the administrative portal on MySolidWorks, SolidWorks will require two startups before recognizing that online licensing is attached to the serial number. The first startup, after going through the standard machine activation wizard, should bring up the prompt seen in Figure 1 and the second should bring up the login screen seen in Figure 2. In this process, a bit in the SolidWorks registry is being toggled which controls the licensing type. We have run into issues where SolidWorks gets stuck on machine activation and continues to launch the activation wizard as opposed to the login screen. In this case, the SolidWorks registry will need to be manually toggled to online activation. The steps below will show how to carry out this process.

Figure 1: Serial Number Set to Online Licensing Error

Figure 2: SolidWorks Login Screen

Manually setting online licensing in the data registry

1. Launch the redgit.exe by either searching it in the search dialog (older operating systems) or using the RUN command and typing regedit in the open bar (Windows 10)

Figure 3: Run Command

2. Expand the HKEY_CURRENT_USER and continue to expand Software -> SolidWorks -> Licenses -> Online

Figure 4: Registry Editor Online Licensing

3. Double click on SOLIDWORKS to set the bit from 0 to 1. The set bits in this registry mean that online licensing is enabled for that specific program.

4. Re-open SolidWorks and verify that the login screen appears instead of the activation wizard.

Login Issues

When someone logs into a profile that is already being used by another station the message shown in Figure 5 should appear. This message should indicate which computer that the profile is currently being used on and provide the option to force them off.

Figure 5: In Use Profile Message

If yes is selected the other user typically has a few minutes before a message appears which prompts them to save before booting them off; however, if for some reason this message doesn’t appear and instead the error message below does (see Figure 6), then follow the below procedure to delete FLEXnet files and fix this issue.

Figure 6: License Limit Exceeded

Deleting FLEXnet files

1. Go to your C: Drive in your file explorer and select your View tab and then Options on the top right

Figure 7: C:Drive & Options

2. Navigate to the View tab in the folder options pop up and select the Show hidden file, folders, and drives bubble

Figure 8: Show Hidden Files

3. Press okay and select the hidden ProgramData folder that now appears on your C-Drive. In that folder then select the FLEXnet folder.

Figure 9: FLEXnet Data & SW_D Files

4. Remove all files that have an SW_D prefix. If any of these files fail to delete, you will need to open task manager and end any SW tasks (some may even be running in the background processes) until it lets you do so.

Logout Issues

The logout/login process has been the most difficult to work with especially with multiple users and workstations. The process of logging out, as seen in Figure 10, has one major flaw being that it is difficult to achieve without physically being in SolidWorks. If you exit out of SolidWorks without logging out (or someone boots you off), SolidWorks automatically retains your login information upon opening (i.e. no login portal). Some issues that the profile retention can cause is, one, accidentally retaining a profile that no longer has a seat of SolidWorks, which brings up the error message seen in Figure 11, and two not wanting to boot someone off who is in the middle of a project with that profile. Before learning the procedure seen below, which walks through manually deleting the login file, we tried using both the modify install login and resetting the SolidWorks registry which both were ineffective. The solution provided is the best option to clear the current profile and bring up the login screen upon re-opening SolidWorks.

Figure 10: Logout Profile in SolidWorks

Figure 11: No License Assigned to Profile Error

Manually Deleting Retained Profile Information from SolidWorks

1. Navigate to your C:Drive and select Users -> [User Name] -> AppData -> Local ->SolidWorks -> Credentials (note: AppData is a hidden folder, go to options and the view tab as seen in the previous example to show hidden folders)

Figure 12: App Data Hidden Folder

Figure 13: UD File

2. Delete the ‘ud.xml’ file

3. Open SolidWorks and verify that the login screen appears; hence, the profile is no longer retained

Resource for Setting up Online Licensing

https://www.cati.com/blog/2018/04/solidworks-2018-admin-portal-online-licensing/

I hope this blog helps with the integration of online licensing for your company needs. We look forward to a new release from SolidWorks in hopes that some of these issues are resolved, but, for the time being, feel free to try out these troubleshooting tips.

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Visualize: Photo Quality Renders

Photo Quality Renders with SolidWorks Visualize

Imagine being able to produce photo quality renders in just minutes without the cost of creating the item in the real world! This blog will introduce you to the powerful, fast world of SolidWorks Visualize and some of the capabilities of the software.

Visualize Introduction

SolidWorks Visualize is a rendering software that was introduced a couple of years ago to users as one of the first standalone software tools to create realistic renders through SolidWorks. Visualize is well known in the industry for the quality renders it’s able to create.

How to Create a New Project

SolidWorks has made creating projects in Visualize very simple from the import process to saving off a final render. One of the first screens that will appear will have tabs set up to view recently worked on projects, some provided sample projects, and recent documents opened within SolidWorks. For creating a new project, it’s as simple as selecting the New Project option highlighted in yellow in Figure 1 below.

Figure 1: Initial Interface

The next step to reaching a photo quality render is to import the desired file with the model to be worked on. Visualize allows the import of many different file types into a new project from SolidWorks files to SketchUp files and 18 others! There are two different ways to import a file into Visualize. The first is to go through the File tab in the top left corner of the screen and select Import from the dropdown list (the same as hitting Ctrl+I). The second way to import a file is to grab it from the folder it is currently in and drag and drop it into the Visualize interface.

Figure 2: Importing Files

After the selected file has been imported into Visualize, an import settings window will appear and allow the user to define what happens to the imported file. These options will vary from person to person as to how they want the file imported. It depends on the size of the imported file, how many components there are in an assembly, and things of that nature. There is also the ability to deselect some of the import setting tabs if none of this information is needed for the final render.

Figure 3: Import Settings

Now, we will describe each tab with a basic overview of what each is trying to accomplish.

Geometry – the focus of this tab is to decide how the imported files will act. You can choose to have the entire imported file change colors/position at once, or it can be refined to allow each individual component of an assembly gets its own color or to move independently from the rest.
Appearance – source model appearances can carry over from the original file if desired. There is also the option to locate the missing textures and to add specified paths for textures.
Cameras – any saved camera views from the original SolidWorks CAD file can be carried over from the SolidWorks software as well as animated cameras from FBX file formats.
Scene – this tab allows to either enable or disable imported environments or backplates from the SolidWorks file.
Decals – this tab allows for the option to import decals from the original SolidWorks CAD file.

Adding Colors to the Model

Once everything has been imported into Visualize, there is now the part where creativity takes over! There are many options as far as what sort of color that can be added to the model, from basic, flat colors to more complex appearances such as a soap bubble appearance to heat treated titanium. One thing to notice is up in the top-right corner there are two tabs: one saying local and the other saying cloud. The local appearance tab is full of appearances that are that are included with the downloaded software. There are still many options for appearances that can be used with this. The cloud appearance tab allows the user the ability to select any appearance or color from the full online library as well as the local appearances. The cloud appearance tab is where many of the more unique options will be located.

Figure 4: Appearances

SolidWorks has made the process of adding colors to the model very simple and easy to do. Once the desired appearance has been located from the palette, all that is needed is to click and drag the appearance to the specific part of the model to apply that specific color. If the chosen appearance isn’t quite correct, there is also the option to adjust and refine them to get the exact desired color. There is an included color picker to select a color from anything on the screen. Also included are sliders to manually go through and slide through all the colors. If the custom created color is something that can be used for other projects, there is the option to save it in a user-specified folder for use later. This is done by selecting the ‘Export’ option in the top-right corner and selecting ‘Save Appearance’.

Figure 5: Custom Appearances

Creating the Final Render

With all the appearances applied and the model all squared away, the final render can now be created to show-off the photorealistic renders. This can be done by selecting the output tools tab at the top-center of the screen.

Figure 6: Output Tool for Final Render

There are many different options to create the final render such as choosing the size of the end photo, the resolution, and whether the software will use the CPU, GPU, or a hybrid of the two. First, select the file name and then map which folder the final render will be saved in. Next is choosing the image format. There are things like if the file is to be saved as JPEG, a BMP, or something like a PNG. No matter which option is selected for the size, the software will scale the photo simultaneously to prevent the size from being too wide or too tall and thus preventing the final render from being out of proportion. Right below size is the resolution option, which determines how many pixels there will be per inch or per centimeter depending on which option is selected. One general rule here is the higher the resolution, the smoother the image will be in the end. Finally, the last options to be adjusted are the render settings. The renderer selection gives three options to how the final render will appear; preview being the lowest quality, fast being a little better than the preview, but not the best, and accurate which will yield the best results. Render mode will only appear if the accurate mode is selected. Render mode allows the user to choose whether they want to set a certain number of passes with the quality option or if they want to set a time limit. For the quality option, however, many passes that are inserted, the software will continually do a render pass no matter how long the time until that final number is reached. The time limit allows the user to set a certain amount of time and when the time is hit, the render will stop no matter the quality at that time.

Figure7: Output Tools

Summary

With all this being said, you now have the tools and basic abilities to create these high-quality photos for marketing your product, helping pitch your design, and just creating cool photos to show friends and coworkers. It may take some time to get everything dialed in to show exactly what is intended, but with time these renders can be created quicker and better than before.

Figure 8: Final Render

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SolidWorks: Displaying and Deleting Relations

Displaying and Deleting Relations

Dimensions are used to define the geometry of sketches or some feature commands. The key purpose of dimensions within the modeling phase of a project is to fully define the part. Relations within the sketching phase do the same thing as dimensions,, without all the hassle of clicking each individual line. SolidWorks at times will include relations automatically if the sketch was done properly. Continue reading on for a How to on display and deleting these relations.

Displaying Relations

Adding relations to a sketch will add a level of constraint to the line or geometry selected and it cannot break or change unless the relation is deleted. In other words, relations override dimensions and will always stay true to the relation until deleted. In the initial stages of creating a sketch, relations will appear in two forms: yellow and white. The white box that appears when adding geometry acts as a reference relation; however, does not add the relation. The yellow box means the relation will be added to the sketch and will be defined with the given relation.

Figure 1: Reference vs Defined Relation

Viewing the relations of a single line or point can be done by clicking on the desired line or point. To the left of Figure 2, the properties manager of the SolidWorks interface which will show existing relations, parameters and give the ability to add relations. In addition to the property manager, the selected geometry will display the relation as well.

Figure 2: Relation Properties

Moving forward to showing the basics of relations within SolidWorks, adding the relations is just as simple as displaying the relation. To make the line shown in Figure 2 vertical without adding a dimension can be done by selecting the line and clicking the vertical icon either in the property manager or the initial pop-up when first selecting the line.

Figure 3: Adding Relations

Enabling the vertical relation will turn the line that was once on an angle to straight up and down; plus, the line will now be defined in the vertical direction.

Figure 4: Relations vs Dimensions

Adding relations can save time and space within the modeling interface by not cluttering the screen with excessive dimensions. Another reason relations are favored more than dimensions is the ease of mobility. Having sketches linked to one another will ensure lines are colinear with each other and equal.

Figure 5: Sketch Relations

To view all the relations in a sketch, select the Display/Delete Relations Icon in the sketch tab in the SolidWorks Command Manager.

Figure 6: Display/Delete Relations Icon

Delete Relations

There are two ways to delete relations within SolidWorks; within the properties manager or on the line itself. Select either the relation box on the sketch or the existing relations name on the properties tab and hit the delete key to delete the relation.

Figure 7: Deleting Relations

Relations to Surfaces

Often, Extruded Cuts, Hole Wizard, or Extruded Boss/Bass among other features are used in relation to the edges of surfaces. The key modeled below will need a circle cut out of the metal for the key ring to go through. Using relations will ensure the circle cut will be centered and in the correct location even after dimensions are changes.

Figure 8: Hole Relations

To select multiple lines, midpoints, or intersections the “shift” key will need to be held when making each selection. Upon selection all the desired points to add relations too, the relations pop-up will appear to define the desired relation.

Figure 9: Fully defined Hole

The hole above is now fully defined in relation to existing surfaces, and when the surfaces move the hole will move in relation to the surfaces. Changing dimensions is a common thing in the engineering industry so have the least number of dimensions can help save time in the long run along with having a clean interface.

Figure 10: Changing Dimensions

Reasons to Add Relations

Relations save time with complicated models, the more dimensions a model means the more challenging it will be to change dimensions and features. The relations will stay true with dimensional changes as seen with the hole above. Modeling with relations over dimensions will take some practice, but over time, they will become second nature and aid in design efficacy and less opportunity for mistakes. Having to change one dimension and the whole model will change in relation is much easier and faster than having to change multiple dimensions.

Glad we could help! Thanks for reading Perception Engineering’s blog. If you have modeling questions or need aid in your projects, our engineering team may be able to help. Have you signed up for our weekly blog postings?

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SolidWorks: Pattern Driven Components

Pattern Driven Components

Some of the most time-consuming work that can be done in SolidWorks is inputting multiple purchased components into an assembly. With all the individual components come individual mates that need to be placed on each component to fully constrain them to the assembly. However, this blog will teach you about the Pattern Driven Components command in assembly’s that will allow one component and its mates to be copied and placed into all holes/features that are the same!

Getting started

The Pattern Driven Component command is only found inside of an assembly file. On the toolbar click on the assembly tab, scroll over to the linear components pattern command and click the down arrow, on that drop-down menu will be the Pattern Driven Component command, as seen in Figure 1.

Figure 1: Command Location

An important thing to note is that the Pattern Driven Component command will only work with features created by the Hole Wizard command. If you are unfamiliar with the Hole Wizard command check out the Hole Wizard blog post!

The Correct Features

For this blog, a block containing 8 holes all the same size will be used as seen in Figure 2. For this example, the holes are threaded and are in Metric units, however, the features can be of any type as long as they are created with the Hole Wizard command. Also, the holes do not need to be in line with each other or even on the same face! The holes may be placed in whatever orientation is necessary.

Figure 2: Example Block

Selecting Your Components

Any component can be used and patterned with the command if it has mate relations to the previously created Hole Wizard hole features. A washer and socket head cap screw will be used in this example. These components were chosen from McMaster.com in accordance to the size of the holes created.

Fully Constraining Components

The first component to be placed into the assembly will be the Base Block with the eight holes in it. It is placed on the origin and fully fixed into place. Second into the assembly will be the flat washer that was chosen. It is placed into the assembly and one if its flat faces are mated coincidently with the top face of the block as seen in Figure 3.

Figure 3: First Washer Mate

A coincentric mate is then placed between the washer’s center hole and one hole in the block, this can be any of the holes on the part, at this time a locking mate is also checked to stop the washer from rotating as seen in Figure 4. The washer is now fully constrained to the face of the base block.

Figure 4: Washer fully constrained

First Pattern

Now that the washer is fully constrained and in the correct place, the Pattern Driven Component command can be used. Click on the command to open up its feature manager panel. The first box asks for the component to a pattern, this is the component that was just mated to the face and feature, in this case, it is the washer. The second box asks for the driving feature or component. This is any of the hole features that you want the component to be constrained to. These are shown in Figure 5.

Figure 5: Pattern Driven Component command manager

There is also a box labeled Instances to Skip. By clicking on this box then selecting some of the hole features you can leave them out of the components to be patterned. If the selected seed Position button is clicked, small purple dots will show up on the center of the hole features. If a new seed position is selected the pattern will form in the formation from that seed point, however, it will still be originated from the component that was selected. This is shown in Figure 6.

Figure 6: Seed Component position

Adding more components

Adding in additional components to be patterned is done simply by following the same steps as before. Now a socket head cap screw will be added to this assembly and patterned. Input a new component and fully constrain it to the hole feature. In this case, the screw is given a concentric mate to the hole and the rotation is locked. The shoulder of the screw or the under face is made coincident to the top face of the washer. The screw is now fully constrained in the assembly. The mates are shown in Figure 7.

Figure 7: Screw mates

The same steps are followed as the washer to pattern it across the holes. The screw is chosen as the component and one of the holes is picked for the driving fixture. Click the green check mark to finish the pattern. The final outcome is shown in Figure 8. Another way that the Pattern Driven Component command can be done is by adding both parts onto the same hole and fully constraining them. After doing this it is possible to pattern both components at the same time to all hole features.

Figure 8: Final Outcome

Why use it?

The Pattern Driven Component command is one of the more powerful ones to use, if done correctly, it can save large amounts of time. Not only are the components patterned into all the holes, but the mates of the original component are patterned as well, giving all components full constraints. There is no doubt that this command is used every day in the industry to add in hundreds of components to assemblies whereas it would take hours to put them in one at a time!