What’s New to SolidWorks 2019

With another year coming to a close a new and improved version of SolidWorks has been released, SolidWorks 2019. This new SolidWorks version is full of powerful new modeling tools and various other updates to help bring design and manufacturing closer together. These updates and features cover all aspects of SolidWorks including, Assemblies, Routing, Drawings, PDM, Plastics, Simulation, Visualize, and much more.

Figure 1 – Photo from SolidWorks Event

Updates to Assemblies, Parts, and Drawing Features

 Making large assemblies both run and load faster has been a goal of Dassault’s almost every year. With assemblies growing more and more complex the need for better assembly performance is long overdue. SolidWorks 2019 has done a great deal to fix this issue by taking computing stress off the CPU and sharing it with the computer’s graphics card. This allows for quick and seamless assembly manipulation. 3D textures can now be applied to 3D models. This process used to take many features and a large chunk of time to add in a simple feature like knurling. Now all the is needed is textural appearance and the use of the new “3D Texture” tool to create complex surface geometries quickly and easily. As for drawings, SolidWorks 2019 allows cell border thicknesses to be changed individually for each cell. Opening drawing documents also will now prompt a progress indication to show both number of components and time taken to open the document.

Updates to SolidWorks Visualize

 Setting up a render to achieve picture perfect accuracy can take a long time, and even longer if your session ends unexpectedly and all that work needs to be redone. SolidWorks 2019 offers a new auto-recover option inside visualize to help prevent lost work if the session is closed unexpectedly. Along with the auto-recovery features comes the denoiser option to visualize to help produce faster and more accurate renders. The denoiser is a simple checkbox option to be selected, it allows for fewer passes and faster render time using a post processing technique to filter out unfinished images. 

 Updates to SolidWorks Plastics

 As for plastic part and mold creation some changes do come in 2019 as well. With the new SolidWorks version comes the ability to add geometry based boundary conditions to models. This update allows for features on the model to be assigned as injection locations, control valve locations, and temperature boundary conditions. An enhanced algorithm has been added to allow more accurate and complicated cooling channels to be formed from sketch lines. This new algorithm gives cooling channels an overall better look and greater precision. Mesh enhancements have also been made to SolidWorks plastics. SolidWorks 2019 allows a mesh to be created before a part file has been saved off. Mesh can also be assigned faces, edges, and vertices before creation. Information about the mesh statistics can now also be pulled in 2019 allowing you to view any bad elements about the mesh and much more.

Updates to SolidWorks Routing

 SolidWorks routing has now been updated to allow the creation of partial or fixed length coverings. A “fixed length covering” tool has been added in to allow various locations and segments of the routing to have custom covers. Improvements have also been made to the Routing Library Manager. These updates to the library include displaying only essential tabs that are needed for routing creation, along with increased response speeds when switching through tabs.

Updates to SolidWorks PDM

 This new version of SolidWorks comes with a long list of much needed updates to PDM. First, performance has been improved for handling large assemblies and complex reference structures. This allows for assemblies with a large number of components to be checked in quickly and easily. Conditional notifications have been added to allow predefined conditions to be set and send transition notifications to users and groups. This also allows notifications to be sent dynamically to users based on variables found on the data cards.

Conclusion

 SolidWorks 2019 is bringing a multitude of updates and features to help users bridge the gap between design and manufacturing. It does not seem like it will be long before every tool you need to go from design to manufacture will be available to you in a single program. What was talked about in this blog was only the beginning to some of the updates in SolidWorks 2019. If you would like to dive deeper into some of these new updates or find others that were not talked about visit the SolidWorks site here: http://help.solidworks.com/2019/English/WhatsNew/c_welcome_solidworks_2019.htm?id=9e4cebd3c875458d9bcb529e16b720ab#Pg0

Figure 2 – Photo from SolidWorks Event 2

Written By:

SolidWorks: Forming Tools

Over the years at Perception Engineering, I have modeled and detailed hundreds of sheet metal parts. Often these sheet metal parts will require specific tooling to match the customer specs. Taking to the internet for help on creating tooling yielded minimal results. Having to do my own research to ensure the customers receive the quality parts they requested; I’ve decided to post my finding to help others out.

Tooling Profiles

SolidWorks has included an assortment of default forming tools for sheet metal parts in the design library. Located on the left side of the SolidWorks interface, click on the Design Library dropdown to access the default forming tools.

 
 
 
 
 
 
 
 
 
 
 
 

Figure 1: Design Library

The forming tools can be applied to any sheet metal part by dragging the desired tool on the sheet metal part. For this, I chose the lance & form shovel. This feature can then be fully defined after the tool is dropped on the part.

Figure 2: Forming Tools

The form tooling feature tree will open by default to move the tooling to the correct location. Most tooling positions can be easily adjusted by simply defining the center and rotation angle. If needed the tooling can be flipped too.

Figure 3: Tooling Feature Manager

In the Position tab shown in the figure above, the tooling can be fully defined and the option to add more tooling features can be done if more sketch points are added to the sheet metal part.

Figure 4: Defining Tooling

Figure 5: Tooling

Custom Tooling

At times other customers will require custom tooling. If the customer provid their custom tooling then simply drag and drop as shown above. However, most of the time Perception Engineering must make the tooling to match the customer profile. To do this, open a new part file.

Create a rectangle extrusion large enough to fit the tooling desired, this rectangle extrusion will later be deleted so don’t spend too much time with getting a perfect size.

Figure 6: Custom Tooling Base

Now the custom tooling can be created as you would any other part: lofts, sweeps, extrusions, and fillets to create the customer stamping profile. Be sure that any radii on top of the tooling is smaller than the material thickness otherwise SolidWorks will not stamp the sheet metal. 

Figure 7: Modeling Tooling

The Form Tool can be found in one of two places: search Form Tool in the command search or by going to insert then sheet metal. 

Tooling Profiles

Figure 8: Forming Tool

The Form Tool Feature tree will pop-up and prompt you to select the stopping face. This will ensure the tooling will press up to the desired face forming the sheet metal as specified. Faces to remove will punch holes in the sheet metal with each face selected.

Once all the faces have been specified, the Insertion Point will need to be identified. This point similar to figure 4 will define the tooling within the sheet metal part.

The model can then be saved as a Form Tool File. Select File Save as and find Form Tool (*.sldftp) and be sure to save the file to the design library forming tools folder similar to the default tooling used ealier. 

Figure 9: File Save as

The tooling is now successfully created! Go back to the sheet metal part that needs the tooling and find the tool. Place it on the sheet metal part and define the tooling location as you read above.

Figure 10: Custom Forming Tool

If you have any question, please feel free to contact me via LinkedIn. Thanks for reading the blog!

Written By: 

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.

Written By:

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!

Written By:

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.

Stay up to Date

Thanks for reading our blogs, if you enjoy the content please subscribe to our weekly blog postings. Perception Engineering stays up to date with the latest technologies and techniques and is happy to help answer any questions you may have.

Written By: