Phone Holder

by rypan27 in Design > 3D Design

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Phone Holder

In this tutorial, I will show you how to create a simple angled desk stand using SolidWorks.

The stand has a triangular side profile, a small front lip to hold an object in place, and circular cutouts in the body.

I started by drawing the side profile with the Line tool. Then, I used Smart Dimension to set the exact measurements and angles. After rounding the corners and adding thickness, I turned the sketch into a 3D model using Extruded Boss/Base.

Finally, I used circles and Extruded Cut to create the openings and complete the stand.

This project is a great way for beginners to learn how to use sketches, dimensions, fillets, offsets, extrusions, and cuts in SolidWorks.

Supplies

Required:

  1. Computer or Laptop – A computer capable of running SolidWorks.
  2. SolidWorks Software – Used to design the entire stand.
  3. Mouse – Recommended for drawing, selecting edges, zooming, and rotating the model.

Optional:

  1. 3D Printer – To print the finished stand.
  2. PLA Filament – For making a physical version.
  3. Slicing Software – Such as Cura or Prusa Slicer, for preparing the model for printing.

The main opening diameter and the center positions described below are reference measurements for recreating the model. The other listed dimensions are visible in the modeling recording.

Create a New Part

  1. Open SolidWorks.
  2. Click File → New.
  3. Select Part, then click OK.
  4. Find the Feature Manager Design Tree on the left side of the screen.
  5. Select Front Plane.
  6. Click Sketch from the top toolbar.
  7. Press Ctrl + 8 to look directly at the sketch plane.
  8. Make sure the units in the bottom-right corner are set to MMGS (millimeters).

You should now see an empty sketch with a red origin point in the center.

Draw the Main Outline

We will draw the side profile of the stand using straight lines.

  1. Select Sketch → Line.
  2. Click the origin to begin the first line.
  3. Move your cursor to the right and click to create a horizontal base.
  4. Without leaving the Line tool, draw a long diagonal line upward and to the left.
  5. Click to create the highest point of the stand.
  6. Continue by drawing another diagonal line downward and to the left.
  7. Click to create the lower end of the shorter slanted section.
  8. Draw another short line extending toward the left. This will become the front support.
  9. Draw one final short line upward to create the lip that prevents an object from sliding off.
  10. Press Esc to stop drawing.

At this point, the sketch should look like an open triangular shape with a small hook on the left side.

Do not worry about making the measurements perfect yet. We will adjust them in the next step.

Set the Main Dimensions

Now we will use Smart Dimension to enter the measurements shown in the video.

  1. Select Sketch → Smart Dimension.
  2. Click the horizontal bottom line.
  3. Move your cursor below the line and click to place the dimension.
  4. Enter 85mm and press Enter.
  5. Click the long diagonal line on the right.
  6. Place its dimension and enter 100mm.
  7. Click the shorter diagonal line on the left.
  8. Enter 65mm.
  9. Click the short line extending outward from the left side.
  10. Enter 20mm.
  11. Click the small line forming the end of the front lip.
  12. Enter 8mm.

Your sketch should now contain the main measurements:

  1. Base:85mm
  2. Long diagonal:100mm
  3. Short diagonal:65mm
  4. Front support:20mm
  5. Small front lip:8mm

Important: If a dimension changes the shape in an unexpected way, check that you selected the correct line.

Set the Angles

We will now adjust the stand to the correct angle.

  1. Keep Smart Dimension selected.
  2. Click the horizontal base line.
  3. Hold Ctrl and click the long diagonal line connected to its right endpoint.
  4. Move your cursor inside the angle between these two lines.
  5. Click to place the angular dimension.
  6. Enter 72° and press Enter.

Now adjust the angle at the top:

  1. Select the two diagonal lines that meet at the highest point.
  2. Place the angular dimension between them.
  3. Enter 44°.
  4. Press Enter.

The stand should now have a triangular profile with a 72° lower angle and a 44° angle at the top.

If the sketch flips or moves unexpectedly, check the position of the angular dimension and make sure you selected the interior angle.

Round the Corners

Sharp corners can make the stand look unfinished, so we will smooth the bends using Sketch Fillet.

  1. Select Sketch → Sketch Fillet.
  2. Find Fillet Parameters on the left.
  3. Enter a radius of 3mm.
  4. Click the corner at the top of the stand.
  5. Check the preview. The sharp corner should change into a rounded curve.
  6. Click the green checkmark to accept the fillet.
  7. Open Sketch Fillet again if necessary.
  8. Select the inside corner where the shorter diagonal section meets the front support.
  9. Apply another small fillet.
  10. Repeat for the front lip and the bottom corner where appropriate.

Use the preview to make sure the rounded corners do not remove too much material.

You should now have a smoother side profile with rounded bends instead of sharp corners.

Add Thickness to the Sketch

The outline is still just a collection of lines. We need to give it thickness before turning it into a 3D object.

  1. Stay in the same sketch.
  2. Select Sketch → Offset Entities.
  3. Enter an offset distance of 3mm.
  4. Enable Select Chain.
  5. Click one of the lines in the main outline.
  6. Make sure the entire connected outline is selected.
  7. Check the yellow preview.
  8. If the new outline appears on the wrong side, select Reverse.
  9. Click the green checkmark.

You should now see two similar outlines separated by 3mm.

The space between the outlines will become the solid material of the stand.

Close and Check the Sketch

Before extruding, make sure the sketch contains a closed region.

  1. Zoom in on the beginning and end of the offset lines.
  2. Check whether the offset operation has created closed ends.
  3. If an end is open, select Sketch → Line.
  4. Connect the original endpoint to its corresponding offset endpoint.
  5. Repeat at the other open end.
  6. Use Trim Entities to remove any overlapping or unwanted line segments.
  7. Check that the inside and outside outlines do not cross each other.
  8. Make sure the region between the two outlines is closed.
  9. Click Shaded Sketch Contours to check the result.
  10. The material region should appear shaded.

If it does not appear shaded, look for gaps, overlapping lines, or disconnected endpoints.

Once the sketch is closed correctly, click Exit Sketch.

Extrude the Stand Into 3D

Now we will turn the side profile into a three-dimensional object.

  1. Select the completed sketch.
  2. Open the Features tab.
  3. Click Extruded Boss/Base.
  4. Find Direction 1 on the left.
  5. Change the End Condition from Blind to Mid Plane.
  6. Enter a depth of 75 mm.
  7. Check the yellow preview.
  8. The profile should extend equally on both sides of the original sketch plane.
  9. Make sure the preview shows the entire stand.
  10. Click the green checkmark.

You should now have a three-dimensional desk stand.

The model will have a triangular shape when viewed from the side, a flat base, a slanted back surface, and a small support lip at the front.

Create the Large Circular Opening

We will now create a circular cutout in the large, slanted surface.

  1. Rotate the model until you can clearly see the large slanted rectangular face.
  2. Click this face to select it.
  3. Select Sketch.
  4. Press Ctrl + 8 to look directly at the face.
  5. Select Sketch → Circle.
  6. Click near the center of the slanted face to place the circle's center.
  7. Move the cursor outward and click again to create the circle.
  8. Leave enough material around the circle so it does not extend beyond the edges of the face.
  9. If you want a repeatable reference size, use Smart Dimension to set the diameter to approximately 55mm.
  10. Exit Sketch.

You should now see a circle on the large, slanted surface.

The 55mm diameter is a rounded reference based on the circle's visible size in the recording, not a clearly confirmed final Smart Dimension value.

Cut the Large Opening

  1. Select the circle sketch.
  2. Open the Features tab.
  3. Click Extruded Cut.
  4. Find Direction 1 on the left.
  5. Select Blind.
  6. Make sure the cut direction points inward, through the slanted wall.
  7. Enter 10mm as the cut depth.
  8. Look at the yellow preview.
  9. Make sure the cut passes through the wall and creates a circular opening.
  10. Click the green checkmark.

You should now have a circular hole in the large slanted surface.

If the hole does not pass completely through the wall, increase the depth or use Through All, after checking that the cut will not remove material from another part of the stand.

Create the Smaller Circular Cut

  1. Rotate the model to locate the small front lip.
  2. Select the appropriate planar face at the front support area.
  3. Click Sketch.
  4. Press Ctrl + 8 to view the selected face directly.
  5. Select Sketch → Circle.
  6. Place the circle's center near the edge of the front support.
  7. Draw a circle so that part of it extends beyond the edge.
  8. For a reference size, use a radius of 14mm, equivalent to a diameter of 28mm.
  9. Exit Sketch.

This circle will create a rounded notch in the front support instead of another large opening.

Check that the circle overlaps the material you want to remove.

Final Sep-Cut the Front Notch

  1. Select the new circle sketch.
  2. Open Features → Extruded Cut.
  3. Check the cut direction.
  4. Choose an appropriate end condition, such as Through All, if the cut should pass completely through the front lip.
  5. Look at the yellow preview.
  6. Make sure only the intended part of the front support is removed.
  7. If the preview affects another part of the stand, use Blind and adjust the depth.
  8. Click the green checkmark.

You should now have a rounded cutout near the front lip.

Rotate the model to make sure the new notch has been created correctly.

Inspect the Final Stand

  1. Exit any active sketch or feature tools.
  2. Hold the middle mouse button and drag to rotate the stand.
  3. Look at the model from the front, back, top, and sides.
  4. Check that the bottom surface is flat.
  5. Make sure the front lip is connected to the main structure.
  6. Inspect the rounded corners.
  7. Check that the large circular opening and smaller front notch are correctly positioned.
  8. Confirm that there are no unintended openings or disconnected bodies.

Your SolidWorks desk stand should now be complete.