Old School Meets New School—A Beginner’s Guide to SOLIDWORKS Weldments
Whether you are coming from a 2D environment, are new to Weldments or just looking for some tips and tricks, this article is for you. I will cover managing your weldment profiles, 2D and 3D sketching, cut list properties and customizing weldment profiles, as well as a few extra tips.
So let’s start with the location of weldment profiles. By default, SOLIDWORKS offers a basic set of profiles with a short list of available profiles and sizes. In Tools→Options→File Locations→Weldment Profiles, SOLIDWORKS points to: install_dir\lang\language\weldment profiles. Figure 1 includes a short list of ansi inch and iso profile styles and sizes.
Figure 1. (Image courtesy of SOLIDWORKS 2016 training manual.)
To download the full list of all SOLIDWORKS Weldment profiles, go to your Task pane and click the Design Library tab under SOLIDWORKS Content→Weldments. There you will find zipped-up standard profiles that are already available.
To access these profiles, just Ctrl + click on the icon seen in Figure 2 to download the files. As you can see, many standards are there. You will want to create a folder to hold your standards on your local drive or on a shared network location, to share with other users. In this example, I used Weldment Profiles as my folder name and extracted the ANSI Inch folder under that (see Figure 3).
In Figure 3, you will see a complete list of profiles available when the ANSI Inch folder is extracted, but be careful. Typically, when you extract the file, your program will want to automatically create a folder with the same name. Using Windows Explorer, make sure that you do not have duplicate folders. If you do, your Weldment Profiles will not work correctly when you are trying to select your profile criteria. For example, if you see C:\Weldment Profiles\ANSI Inch\ANSI Inch, move the subfolders up to the first ANSI Inch folder.
Now that you have your profiles extracted, tell SOLIDWORKS where to find those profiles. In SOLIDWORKS, go to Tools→Options→File Locations→Weldment Profiles and add your new location (shown in Figure 4). SOLIDWORKS doesn’t always point to the correct location, so typically I will remove the default location and just add my own.
Now we are ready to begin working with our profiles. Before we actually begin, let’s look at how SOLIDWORKS is built to design weldments. Weldments use sketches to drive the location of your profile, just like a sweep command.
By using a sketch layout, you can drive the location of your profile to “sweep” along the path of the layout, as you see in Figure 5. Once I have added additional paths to my feature, SOLIDWORKS will use a multi-body method, which means that it recognizes each of the pieces as individual bodies. This will allow me to create my entire layout and design everything at the part level. In addition, I can add non-weldment bodies, such as sheet metal, to complete my design right there in the part file. I will also get a Cut list of all of my bodies as well as their properties, just like a bill of materials for an assembly.
How do you lay out your sketches? There are no right or wrong answers. It really depends on which way works best for you. You can choose to work with 2D or 3D sketches, or a combination of both. You can also determine whether you want to lay out your entire sketch profile and then create your Weldment structure, or create your sketches as you go. Working with 3D sketches is a little more work, but with practice, it is a great way to get your entire sketch layout done and also to create unique shapes, especially when you are working with round tubing (see Figure 6).
Using 3D Sketch, you can use the tab button to change the direction of the entities; keep an eye on your triad (bottom left corner of your screen) to assist you with orientation.
From experience, I like to lay out my sketches first, especially if I am using a lot of same-size profiles, to cut down on extra procedures, such as trimming later on in the design. This will also keep my FeatureManager design tree smaller (which, in turn, frees up RAM and keeps the computer from slowing down).
Sketches do not get absorbed into the Weldment feature, so you can use the initial sketch or sketches and select the entities you need as you go.
A couple of neat tricks I learned for sketching: For a simple frame, create a solid extrusion. Filter edges (hotkey is E, or hit F5 to turn on filters) and do a Ctrl + A for Select All. Launch a 3D Sketch and use Convert Entities to get the results you see in Figure 8.
For something more complex that is symmetrical, such as the elements in Figure 9, lay out one side of your sketch and do a surface extrude. Then follow the same procedure: Filter Edges, then Ctrl + A, launch a 3D sketch, convert entities and hide the surface bodies. This is a quick, easy way to get that more complex layout. Remember to turn your filter off before you proceed!
Now that you have determined how you are going to create your sketch layout, it is time to start using the Weldment feature. Right-click your CommandManager tabs and check the box for Weldments, then click Structural Member. Here you will define the following:
- The type of standard: ANSI Inch, ISO, JIS, etc.
- The type of profile: Tube (square), I beam, c channel, etc.
- The size
You can also create your own profiles. I like to create my own custom folder under whatever standard I am using (for example, ANSI Inch\Custom Profiles) and add my profiles there. If you have a profile that is similar, don’t be afraid to do a “Save as” to one of the existing profiles and modify to your needs. The profiles are SLDLFP file types, which stand for a SOLIDWORKS library feature part. This saves the hassle of trying to remember the correct file format when creating your own.
Now that I have my Weldment member feature defined (Figure 10), it is time to start selecting entities. After your first entity selection, you will get a preview of the profile following that entity path, and now you can continue to select entities. There are some rules when selecting entities to be part of the same group. The following are the general rules you need to follow:
- Connect end-to-end
- Can be disconnected but are parallel
- Cannot select more than two entities sharing a vertex (connected)
When additional entities need to be selected, click on the New Group button and continue to add them. As long as they are all the same type and size, you can have one feature representing multiple bodies. I always try to use the old general SOLIDWORKS rule: If you are not seeing a preview, then the Weldment (or other general function) will fail. However, just click the New Group and you can keep going. Figure 11 and Figure 12 are an example of three groups. The first group is the front four entities (Figure 11), the second group (Figure 12) is the back four entities and the third group is the top two rails.
Figure 11.Figure 12.
Another thing I can control in the Weldment properties is the corner treatment. I can apply an end miter or end butt to all corners by selecting “Apply corner treatment” (see Figure 13).
This will drive the corners overall and allow you to add uniform weld gaps and your desired dimension. However, you may find that you need to control corners individually to get the results you are looking for. At any time, you can click on the pink dot in the corner and determine how you want that corner to behave. This allows you to mix and match end miter and end butt corners throughout the design.
Notice in Figure 14 that SOLIDWORKS is automatically trimming weldments as additional groups are added. It is the order of the selection that drives this, so the bodies from Group 1 will automatically trim the body from Group 2.
You can also define the order of a trim to drive what order the trim happens using the Trim Order in the Corner Treatment. In Figure 15, the corner was switched to an end miter trim and the order changed to get the desired results.
You can continue to add new groups and select more entities as long as I am continuing to work with the same type and size weldment. This is one advantage of having my complete sketch layout prior to starting the weldment structure: letting SOLIDWORKS do the work of automatically trimming my corners. Since there is one feature in the FeatureManager design tree, I can globally change the size for all of the groups at the same time.
In addition, I can easily control the profile by mirroring it, using a sketch or edge to align the profile, rotating the profile and, last but not least, locating the profile. So what does that mean?
When a group is selected and I click on the Locate Profile button (Figure 16), SOLIDWORKS will zoom in to the original profile and allow me to pick any endpoint or manual point added to the profile to determine where the profile is connected to the sketch entity. In Figure 17, I change the profile location from the center of the profile to the virtual sharp of the profile. This is going to allow me to use my sketch layout as the center, inner dimension (ID) or outer dimensions (OD) of my weldment structure, or I can mix and match as I go.
So what exactly is driving the weldment profile? Basically, this is a simple 2D sketch with a closed sketch profile and additional points that allow me to have more location points (see Figure 18), and a description for a custom property. This will popluate my feature tree with that information as well as my Cut List description (see Figure 19), which I will cover later. You can also add information like Material to these profiles. Note the Library Feature symbol on Sketch1 in the tree in Figure 18.
Figure 18.Figure 19.
Now it is time to add a different size Weldment profile. I click on the Structural Member icon, select my new parameters and start choosing entities and groups.
When a second weldment feature is created with multiple groups (Figure 20), it will still auto-trim, based on group order, just like the first weldment feature. However, manual trimming must be done to clean up the new weldment feature to fit to the first weldment feature that was created. You can see in Figure 21 the interference of the new weldment structures. This is where the Trim command comes into play.
The Trim icon located in the Weldments tab is fairly easy to use. You can trim using faces, planes or existing bodies. In this case, I can use the existing square tubing to trim up the new rectangular structures and cut them to the proper length. The preview and callouts in Figure 22 will help you keep track of what is being kept and also what you are using to trim.
The end result seen in Figure 23 shows the finished result of the trimming.
As I complete the design with some additional weldment features, let’s take a look at the FeatureManager design tree and the weldment bodies.
Figures 24, 25 and 26.
Figure 24 is the end result of my structure. As you can see in Figure 25, the FeatureManager design tree includes all of my weldment features defined by type and size for each. As you expand the Cut list (Figure 26), SOLIDWORKS puts items together that are identical in shape, size and length.
In Figure 27, I have my Document Properties settings to use the description property for naming the weldment items under “Rename cut list folders with Description property value.” This makes it easy to see what the sizes and the quantity of the identical items are.
Next, I want to take a look at the Cut List properties—basically, what is available to include in my Cut list at the drawing level. After adding a material to the part (Plain Carbon Steel), I can add individual materials to any body. Holding Ctrl and selecting the bodies under the Item Folder and select Edit Material adds the material directly under that Item folder. In Figure 28, AISI 304 was added to four of the members.
Now let’s look at the Cut-List Properties command. Right-click any item folder and select Properties. By default, the Cut List Summary (Figure 29) includes items such as cut length (LENGTH, Description, MATERIAL and QUANTITY).
The Properties Summary tab (Figure 30) can be used to evaluate specific properties. This allows me to verify that all of my information is complete, e.g., that my materials are being called out correctly.
The last tab, as seen in Figure 31, is the Cut List Table, which gives me a preview of my cut list for a drawing. In this scenario, the default Table Template is called the cut list.
It is amazing that this is all done at a part document level. Now it’s time to create the drawing. Hint: Before you make the drawing, make sure to hide your sketches using View→Hide/Show→Sketches, so they don’t appear in the drawing.
Once I have added my drawing view, I can insert my Weldment Cut List (Figure 32). All of the information that was available in the parts file is available as columns here.
Make sure to check the Cut list item property radio button in Figure 33 and select your desired property from the drop-down menu. You can right click and save the template to re-use for other weldment drawings.
The last step is to balloon your model to pull the ITEM NO. from your Cut list table (Insert→Annotations→Auto Balloon), just as if you were working with an assembly drawing. In Figure 34, you now have everything you need to create this weldment and it is now ready to go to production. I highly recommend signing up for a SOLIDWORKS Weldments training course with your local reseller to learn more.
About the Author
Cami L. Florence is a support engineer leader. As a member of the Fisher Unitech team for the last nine and a half years, she currently trains and does technical support for SOLIDWORKS. She started working with SOLIDWORKS back in 1997 and achieved her CSWE in 2013. She had the pleasure of giving her first SOLIDWORKS World presentation in Dallas at SWW16.