Making a Model Library

Custom design libraries can be a great cost savings for many companies. They allow any user to drag and drop standard components into their designs or use custom profiles for weldments. Libraries may have the parts and/or profiles created in-house or downloaded from online sources. If downloaded from an online source, you will first want to verify the design (and your rights to use it) prior to converting it to a library part.

SOLIDWORKS does have extensive library files for weldments, yet you may require speciality items that are not included. These are easy to create and add to a network drive where any designer in your organization can access them. For example, you may want to start by designing custom sheds using standard lumber profiles that are not included with the software. Designing framed walls as a weldment will make the work quick and allow for lumber sizes to easily change. For example, Figure 1 shows a shop I want to build that was created as a weldment so that I could easily create a material list for each wall.


Figure 1. Author’s future workshop (pending wife’s approval).

Each wall of the final shop assembly is a weldment and created from custom lumber profiles added to my design library as shown in Figure 2. By using a weldment design, I can easily change the lumber size while maintaining the outside dimension of my building and quickly getting a new weight of the structure.


Figure 2. North-side wall of future shop created as a weldment profile.

The lumber profiles can be downloaded here. They can also be created by following these steps.

1) Start a new inch part.
2) In the front plane, create a new sketch.
3) Sketch a center point rectangle that is locked to origin as shown in Figure 3.image005

Figure 3. Center point rectangle with points added at each segment’s midpoint.

4) Dimension the rectangle 1½ x ¾.
5) Add four points—one to the midpoint of each line segment. (These will be used to position the profile in a weldment.)
6) Right-click on each dimension and uncheck “Mark For Drawing.”
7) Exit the sketch.
8) Set the material to “Pine.”
9) In the network drive or shared location where you would like the profiles saved, create a new folder—I called mine “Workshop.” This may be done through Windows Explorer.
10) In this folder, create another new folder. I called mine “Lumber Profiles.”
11) One more time—create another new folder within this last folder. I called mine “Pine.”
12) From the drop-down menu, select “File, Save As.”
13) Navigate to the file path you created in steps 9 to 11. In my case, I navigated to “E:\Workshop\Lumber Profiles\Pine.”
14) Name this profile “1×2.”
15) From the “Save as type” dialogue, select “Lib Feat Part.”
16) If you receive a warning as shown in Figure 4, select “No.”
17) Save the 1 x 2 profile, and double-check the folder is still the correct one.
18) In the feature tree, right-click on your “Sketch 1,” select “Add To Library” and save the part.

image007Figure 4. Dialog box about the library part features.

Your feature tree should look similar to Figure 5, with the “L” over the sketch and the library symbol at the top left of the feature tree.


Figure 5. Feature tree appearance for the 1 x 2 library lumber profile.

Edit the sketch to the size of the next lumber profile you wish to create. Exit the sketch and repeat steps 13 through 18.

Now the software must be set up to look in this location for the new profiles. From the drop-down menu, select “Tools, Options.” In the “System Options” tab, select “File Locations.” Click on the “Show folders for” drop-down to open the selection window, scroll down and select “Weldment Profiles.” Select the “Add” button and navigate to where you saved your profiles. Select the first folder you created. In my case, I select “E:\Workshop” and “OK.” Select the folder—now located in the list as shown in Figure 6. Then select “Move Up” until the folder is at the top of the list.


Figure 6. System Options window showing the added lumber profiles location as a selection option for weldment profiles.

Select “OK” to close the System Options window.

These standard lumber sizes can now be selected as structural members for any weldment by any designer who has access to the network drive where they are stored. Each user will need to edit their system options as outlined in order to use these profiles. Any custom structural member library may be created by following these steps.

To see a video of another custom profile being saved to a library, watch this video.

You may also have standard parts that are used frequently within your company and wish to save these as library items that can be dragged and dropped into an assembly like many standard components.

To do this, first create a folder on your network drive where you would like the parts stored. I called mine “Facia.” Save your part(s) to this folder. On the right side of your screen, select the Design Library as shown in Figure 7.

image011Figure 7. Selecting the Design Library.

Click the “Add File Location” icon as shown in Figure 8.

image012Figure 8. Adding a new library file location.

Browse to where you created your new folder, select it and then click “OK.” You can now drag and drop any item in this folder into any assembly or create a derived part.

Again, any designer wishing to access this library folder will need to add the shared location to their computer. Parts may also be added to this or any other library folder by starting with the part open. Then click the “Add to Library” icon as shown in Figure 9.

image013Figure 9. Adding a new part to an existing library folder.

Next, select the items to add to the library folder by clicking on them in the graphics area or from the feature tree, and accept these selections by selecting the green check mark.

By following these steps, any part or assembly may be added to an existing library folder or to a newly created folder.

Downloaded parts may also be added to a design library; however, you should first check them for errors. To check a downloaded, non-SOLIDWORKS part, follow the steps as outlined below.For SOLIDWORKS parts, ensure that a good design intent was followed and that there are no under defined sketches, and add the part to the library as described earlier.

1) Download and open the part.
2) If the part is a generic solid file type, such as a STEP file, you will be prompted if you wish to run diagnostics on the parts, as shown in Figure 10.If you are not prompted, select “Tools, Import Diagnostics” from the drop-down menu.

image014Figure 10.Prompt to run diagnostics on a part.

3) Select “Yes.”
4) The part may be fine or it may have faulty faces, surfaces or gaps, as shown in Figure 11.

image015Figure 11.Import Diagnostics tool showing a faulty face.

5) Select the faulty item from the list to display the area of the part with the issue.
6) Select “Attempt to Heal All.” If the part cannot be automatically repaired, you will need to delete the faulty face and repair the gap. The direct editing feature works great for such cases. If the fault was healed, the software will display a message highlighted in green indicating that the faulty geometry no longer exists, as shown in Figure 12.


Figure 12. Import Diagnostics tool displaying the message that all faults have been corrected.

7) Exit the Import Diagnostics tool.
8) Save the part.
The part may now be added to a library as explained earlier.

The creating of custom libraries can save any company significant costs and design time because time is not wasted recreating the same parts again and again. These library parts can also be the starting point for similar designs, again saving time and money. Once the custom parts and/or profiles are created, they can quickly be utilized in any design.

About the Author


 Fred Fulkerson is a graduate of the Faculty of Education, University of Western Ontario, and of the general machining program at Conestoga College in Ontario. He is a Canadian Red Seal certified general machinist and CNC programmer and a certified Mastercam and SOLIDWORKS instructor.

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