Using Photos in the Design Process

Oh no! The handle on my outdoor spigot broke!

I need to make a nice smooth handle so my wife and I won’t cut our hands anytime we go to water the garden. The handle has an odd outside shape and custom cutout area that I will need to fill in.

In today’s blog, I’m going to show you how I was able to take some photos with my cellphone and bring them into SOLIDWORKS. I was then able to trace the perimeter of the photo into a SOLIDWORKS sketch. That gave me a great foundation for my layout sketches, which simplified the overall process of creating a 3D model.

Step1: Taking and Transferring the Photos

Let’s start with some basic guidelines for working with the photos. You’ll want to have a nice crisp outline of the physical part. Be sure to hold the camera still and ensure the part is in focus. If possible, use a backdrop of a contrasting color. I sometimes place a bright piece of paper behind the physical part as my backdrop.

Be aware of perspective. You can sometimes get less perspective, and better results, by standing back a bit from the physical part.


Standing too close to the physical part can cause undesired results due to perspective.

Next you will need to transfer the photos to your SOLIDWORKS workstation. There are two methods I use to do this. The first is via USB cable.


Transferring photos to a computer using a USB cable.

This is the method I use if I have a lot of photos of the project. The second method I use is transferring the files wirelessly via online storage. I use this method when I only have a few files to transfer.

Step 2: Post Processing the Images

After l get the photos onto my computer, I open the files in some type of image editor like Photoshop or MS paint. I personally like to use the free program Paint.net.

After I get the files into the post processing software, there are three things I want to address before using the images in a SOLIDWORKS project: cropping, file name and file size.

Cropping the Images

I start by opening the image and using a crop command to remove any unnecessary data from the background. Remember, to avoid perspective, you had to stand back away from the physical part. This means you will likely have a lot of excess “background” in your image. Remove this background to keep the image clean and tight using a crop command.


Cropping the images of your physical part.

Renaming the Images

After cropping the image, I like to do FILE>SAVE AS to give the images a more usable name. By default your cellphone will give the files a generic file name, often based on the date and time. I like to rename my images to something more usable like “FRONT VIEW” or “RIGHT SIDE.”


Renaming your images to something more usable.

Decreasing the Image Size

We should also be looking at the file size of the image. Most cellphones will take a high-quality image by default. This can lead to a very large file size. You want the image to be crisp and clear in SOLIDWORKS, but you want to balance that with an appropriately sized file. By using a RESIZE command and then re-saving the image, you can decrease the image size, which will decrease the file size. I make it a goal to keep my files between 500kb and 1mb.


Reducing the file size before using these images in a SOLIDWORKS project.

Step 3: Adding the Photos to a SOLIDWORKS Project

We are now ready to start using these photos in a SOLIDWORKS project. I like to start by taking a reference, or overall, dimension from the physical part. For our model we are going to say that the overall height is 59mm, based on the following photo.


The overall height of the physical part is 59mm.

Creating a Layout Sketch

I’m going to start a new part file in SOLIDWORKS and create a new sketch on the front plane. This sketch is going to contain a single circle with a diameter of 59mm. This sketch will be my LAYOUT sketch. I will size the image to match this 59mm circle. I’m also going to add eight “spokes” to help align the image to my SOLIDWORKS project.


Creating the initial layout sketch in SOLIDWORKS.

After creating this geometry I will exit the sketch and rename it in the feature tree. Next I will right mouse button click on the name of the sketch and choose SKETCH COLOR from the menu. I want to change my sketch from the default grey color to a color that will be a little easier to see when the image is added to my model. For this sketch, I will use yellow.


Renaming the sketch and changing the color of the sketch from the default (grey) to yellow.

I next start a new sketch. This will be the sketch where I add the image to my model. I choose the command TOOLS>SKETCH TOOLS>SKETCH PICTURE and then choose to add the picture named FRONT VIEW.


Creating a new sketch and using the command TOOLS>SKETCH TOOLS>SKETCH PICTURE to add the front view of the spigot.

We can see in the above image that our original yellow layout sketch is much smaller than our imported image. This means we need to resize our image. We are going to start by using the sketch picture scale tool.

Using the Sketch Picture Scale Tool


The SOLIDWORKS sketch picture scale tool.

In the above image we can see the SOLIDWORKS sketch picture scale tool. By using this tool, we can re-size our image to match our design.

The tool consists of three elements: a magenta dot on the left side, a thick blue centerline and a magenta arrow on the right side.


The four steps of using the scale tool.

In the above image we see the four steps involved in using the sketch picture scale tool. We start by dragging the left magenta dot and placing it on the far left of wheel of our spigot, as shown in step 1. We then drag the magenta arrow and place it on the far right of the wheel of our spigot, as shown in step 2. After we drop this arrow, we are prompted to input a dimension. We will enter 59mm as shown in step 3, since this is the overall size of the wheel of our spigot. After we press enter, we will see the results shown in step 4. The sketch picture was scaled so that the distance from the magenta dot on the left to the magenta arrow on the right represents 59mm. This should get us close to the appropriate scale of our layout sketch.

Turning off the Scale Tool

I now have the image scaled close to the appropriate size, but I want to do some final subtle adjustments. Unfortunately we cannot drag the corner of the image when the scale tool is enabled.


When the scale tool is enabled, we cannot drag the corner of the image to resize.

I like to first move the image close to the origin and then uncheck the option for “Enable scale tool.”


Move the image close to the origin, then uncheck the option for “Enable scale tool.”

Final Adjustments to the Image

Now that we have the image close to the origin, we need to make some final adjustments to get it aligned with our layout sketch. I can drag the image to relocate it and grab the corners to resize the image. I can also use the rotation angle to ensure that the spokes of the image are aligned with the spokes of our layout sketch.


Making our final adjustments to the imported photo.

As we can see in the above image, we moved and resized the image until it matched the size of our 59mm layout circle. We also adjusted the rotation angle by 1.4 degrees to ensure that our spokes were aligned. Lastly, we adjusted the overall transparency of the full image to about 40%. This is a little trick I like to use, as it will make it easier to work with the image and our 3D model.

Using the Imported Photo to Create Sketch Geometry

We can now exit the SKETCH PICTURE command using the checkmark. We can also exit this sketch and rename it to something like “IMAGE – Spigot Front.”

We now begin a new sketch and create the geometry for the first “wedge” of our 3D model.


Creating sketch geometry based on the image of the physical part.

For the 3D model I decided to add some clearance and go with a diameter of 63mm. I used the image to help guide the sketch of the arcs to match the existing physical part.


Creating sketch geometry based on the image of the broken cutout area of the physical part.

I exit the sketch of the “wedge” and begin a new sketch. This time I use the photo to help guide me in the creation of geometry representing the broken cutout area of spigot handle. This geometry would be difficult to capture using traditional measurements. By having a photo of a physical part, it’s easy for me to create geometry that matches the broken area.


Using the layout sketches to drive extrude features of the 3D model.

Now that I have these layout sketches complete, I’m ready to start creating the 3D model. The image above shows the first few features created using the extrude command in SOLIDWORKS.


Adding some final features to the 3D model.

I add some final features to the 3D model, and this thing is looking pretty sweet.

3D Printing and Testing

Now that I have the 3D model complete, I’m ready to send it to the 3D printer.


Creating a 3D print of our new spigot handle.

Now for the fun part—testing it to see if it fits.


Testing our 3D print to see if it fits on the handle and matches the broken section.

I am happy to report that it does fit. It fits like a glove. SUCCESS!

Conclusion

In today’s blog we took a look a common challenge: We had to create a SOLIDWORKS 3D model of an object with a shape that is difficult to capture using traditional measurements. By taking a photo of this physical object and bringing it into SOLIDWORKS, we were able to use this photo as a guide for our sketching process. This made the process much more straightforward and left us with a result that fit just about perfectly onto the existing physical model.

Remember to first create a layout sketch with the appropriate size and then scale your photos to match this size. Use the scale tool first, but then turn it off for fine adjustments. Use the rotate tool to adjust the angle of your imported photos. You can set the images to transparent to make them a little easier to work with.

Good luck, and I hope you too can save time on future projects by following these steps!

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.

*Source: Engineers Rule