Using a Company Logo in SOLIDWORKS
In the world of tech support, one of the more common questions we receive is “How do I work with a company logo in SOLIDWORKS?” This question comes in various forms, including “I want to show a company logo on a part, and I want it to display in the drawing view” or “I want to include our company logo in a drawing title block. “In this blog we will take a look at some challenges users face when working with company logos, and some best practices to ensure that you get consistent and reliable results.
Our Fictional Company Logo
In this example, we are going to work with a fictional guitar company, “Toby’s Guitar Co.” Our goal will be to use this company logo on our title blocks in drawings. We also want to create a cut extrude of this logo to use on the chrome neckplate of the guitar.
Getting Started with a Logo Image
To get started we should first try to get the highest quality image of the logo we can find. This might be from the company website, marketing material they provide or from a photograph of the logo.
The ideal scenario happens when the company has, and is willing to share, a DXF or DWG of its company logo. When this happens, it saves us quite a few steps. More often than not, companies will only share an image with you. But it’s always best to ask the company if they have a DWG, DXF or vector image of its company logo before recreating it.
We were able to reach out to the marketing team of “Toby’s Guitar Co.” and secure a high-quality image of the logo, as shown in the image above. Now we want to use this image in a few areas in SOLIDWORKS.
Some Things Might NOT Work
Let’s start by addressing some techniques that might not work for you. Maybe you’ve run into some of these scenarios in the past. The first of these techniques is to use this image in a title block in a drawing.
When working in drawing mode, we can simply select INSERT>PICTURE and add our company logo to the title block. This works great and is a simple process to follow. When using this method, we occasionally run into issues downstream.
The first issue we run into occurs when we save our drawing as a DXF or a DWG.
Depending on the format of the image, exporting the drawing to DWG or DXF can sometimes yield undesired results. In the image above, we can see that the image did not translate through to the DXF, so we were left with an incomplete title block. (This doesn’t ALWAYS happen, but it is one little thing that can cause a hiccup).
Sometimes when we add images to drawings, we choose to use linked images. This can be an elegant solution because if the source image changes, the title block automatically updates. When the link to these images is broken, or the source files are no longer found, we can end up with an incomplete title block because the company logo no longer shows properly, as illustrated in the image above. (Again, this doesn’t ALWAYS happen, but it is another little thing that can cause a hiccup).
Next let’s talk about decals.Decals are an amazing tool in SOLIDWORKS and a great way to show a company logo on your parts.But decals won’t show in a traditional drawing view, as shown in the image above. There may be times when you want to show the manufacturing team exactly where the company logo is supposed to be located right on the drawing view.
Converting Your Company Logo to SKETCH Geometry
We’ve now covered a few things that might not work when using a company logo in your SOLIDWORKS projects. These tools are all great tools, and they all have their place, but sometimes we want to go the extra mile to ensure that our company logo always works and that our entire manufacturing process can use the company logo geometry. In these cases, the best thing to do is to create a new sketch of the company logo.
Sizing Up Our Logo
We’ll start by creating a brand new model. Once we create this model, we’re going to create a simple sketch representing the overall size of our logo. Later in this blog we will see how easy it is to resize our logo, once we make it a sketch block. For now we are simply going to choose to make our logo 200mm wide.
After creating this we can exit this sketch and begin a second new sketch on same plane. We can use the command TOOLS>SKETCH TOOLS>SKETCH PICTURE to insert our company logo, as shown in the following image.
After inserting this image we can resize the logo to match the line created in the previous sketch.I also like to toggle the option for FULL IMAGE TRANSPARENCY, and set it to about 50 percent.
Using Splines to Trace Our Company Logo
Now the fun part begins—we exit this sketch of the company logo and begin a new sketch. I like to take certain areas of the company logo and recreate them one sketch at a time. This helps prevent accidently moving part of the sketch, since we often leave parts of the company logo sketch as under defined geometry.
We’re going to start with the snake shaped “S” in the company logo. We exit the current sketch and begin a new sketch on the same plane.
In this new sketch, our goal is to capture and convert the existing logo image into a SOLIDWORKS sketch. This often means working with splines, which we can see in the image above. We want to try to get as close to the original logo as possible. Splines are a great tool to use for shapes that have a lot of curvature. We are now finished with the first section of our company logo, so we exit the sketch.
Working with Text from Our Company Logo
After tracing the curvy element of the logo, I like to begin a new sketch for the next element of the logo.In our case, we are going to next capture the text “GUITAR CO.”
In the above image we can see that we start by using the SKETCHED TEXT command. It can be very helpful to use a construction line and dimensions to define the location of the text. This will give us the ability to make some subtle adjustments to the font size and location, until we get pretty close to a match, as shown in the above image.
Dissolving Our Sketch Text
We now have our sketch text looking pretty close to the original company logo, but now we need to do some fine-tuning. To accomplish this, we can do a right mouse button click on the sketch text and choose DISSOLVE SKETCH TEXT, as shown in the following image.
Using dissolve sketch text actually helps us with two areas of this process. Once the text is dissolved, it becomes individual lines, arcs and splines. This means we can fine-tune the text to match our company logo.
As we can see in the above image, after dissolving our sketch text, we can make further adjustments to match our existing company logo. In our example, the text we selected got us pretty close, but we needed to slightly change the geometry of the letters “I” and “R.” We also needed to change some of the spacing of our letters and the period in “CO.” from a rectangle to an oval.
Being able to fine-tune our text is a huge benefit of using the dissolve sketch text command. The other advantage of using the dissolve sketch text command is that we can now use this text geometry in downstream operations where sketch text cannot be used. The most common tool where this will become an issue is the CONVERT ENTITIES command in sketch mode. When we have sketch text in an earlier sketch, we cannot select this sketched text for a convert entities command. This is a limitation of the software. We can convert sketch text that has been dissolved. This will be very useful when working with company logos.
Converting the Final Part of Our Logo
We are now ready to exit the sketch for “GUITAR CO.” and create a sketch for “TOBY” with the symbol in the letter “O.” We will follow the same steps as the previous section. Begin a new sketch, create some sketch text, get it close to our company logo, dissolve the sketch text, go in and make some final changes.
In the above image we can see that the sketch text was created and positioned so that it is a close match to the original logo. We then dissolved the sketch text and added the final touches to get it to match the original logo more accurately.
Combining the Sketches and Creating a Sketch Block
We now have three sketches representing the different areas of our company logo, as shown in the following image.
To get these three sketches combined into one single sketch, we can begin a new sketch, choose each of these three sketches(from the tree) and launch the CONVERT ENTITIES command. This will convert each of the three previous sketches into the current sketch. As we mentioned earlier, this would not be possible if we hadn’t chosen to dissolve our sketch text.
Now that we have our entire company logo in one single sketch, we want to be able to easily use and reuse this logo. One of the best ways I have found to accomplish this is to create a sketch block using the command TOOLS>BLOCKS>MAKE.
To turn our logo into the block shown in the above image, we can do a window select and select all of the entities in our sketch (the entire company logo). We can then choose TOOLS>BLOCKS>MAKE. This will take all of our selected entities and turn them into a sketch block.
Adding Our Sketch Block to the SOLIDWORKS Library
We don’t want to have to always open this “logo part” whenever we want to use this sketch block. The next step is to add this sketch block to our SOLIDWORKS library.
To add our block to the design library, we can start by selecting our block from the SOLIDWORKS feature tree. We can then go into the TASK PANE, the tabs on the right side of the screen, and choose the DESIGN LIBRARY.We then choose the folder where we want to store the block.In the above image, we have chosen the ANNOTATIONS folder. We then choose the icon for ADD TO LIBRARY, and we finish by giving the block a name.
Adding the Company Logo to Our Drawing Title Block
Now that we have our company logo stored as a block in our library, let’s see how easy it is to use and re-use. We can close all of our open files and open our drawing. In the drawing, we will edit the sheet format and examine the title block. We want to add our company logo to the title block, so we expand our design library and then drag and drop our company logo right onto the title block.
In the above image we can see how easy it is to drag and drop our logo from the design library into the drawing sheet format. But it’s not the right size. The nice thing about blocks is that they are very easy to both move around and resize.
The logo looks great in our title block. We can add some shading to it if we want it solid and, of course, when we export this to a DXF or DWG, we can be confident that the sketch block will come through to the DXF as expected.
Adding the Company Logo to Our Solid Geometry
The last thing we want to show is that we can follow this same process of dragging and dropping the block from the design library to create a new sketch geometry in a solid model.
In the above image we can see that the process starts with us opening the 3D solid model of our neck plate. We then drag and drop our company logo from the SOLIDWORKS design library onto a planar face of our model.This creates a new 2D sketch. Our logo is added, as a block, to this 2D sketch.
Just like with the drawing example, we can scale and reposition our logo to get it into the desired location.
Once we have the logo sized and positioned, we can jump right into a CUT EXTRUDE command, to add our company logo as a 3D feature.
This of course means that the company logo will now display in our drawing, so we can convey to the manufacturing team where the logo is to be located.
When it comes to working with a company logo in SOLIDWORKS, there are a number of different tools we can use. We can add the logo as an image, either in our drawing title block or in our model as a decal. There are some limitations when we use embedded images in SOLIDWORKS projects.
Instead, we can consider taking a company logo and turning it into a true sketch. This often means importing the logo as an image and taking some time and care to properly recreate the company logo as a SOLIDWORKS sketch. Once we have the logo converted into a single sketch, we can use the TOOLS>BLOCKS>MAKE command to create a sketch block and add this sketch block to our design library. This block can then be easily used and re-used on future projects. We can insert this block into the title block of a drawing or use the block as a sketch geometry in a 3D feature on our model.
About the Author
Toby Schnaars is a Certified SOLIDWORKS Expert from Philadelphia, Pa. He has been working with SOLIDWORKS software since 1998 and has been providing training, technical support, and tips and tricks since 2001.