Freecad tutorial – Knob – Product design #101
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Freecad tutorial – Knob – Product design #101


Hello! In this tutorial, as shown in the video, we’ll be making a knob. We’ll start right away. Make sure you’ve started new file, and Part design workbench opened. For each part you create, you’ll have to start the “body”. Body, in general, is a container. Choose to create the body from toolbar, or Task panel. We can see Body created within model tree. Now, you can start new sketch. Select XY Base plane from the panel, or, viewport. Click OK, and you’ll be in Sketcher workbench. Choose Circle. While the cursor is over the dot, and highlighted, click to start the circle. Circle will be automatically constrained to the center. Click again to complete the circle. Notice dot constraint already created. Select circle, and add radius constraint. When radius dialog appears, enter 32mm. Click and drag constraint, to move it to a better position. Use mouse wheel to zoom out. And close the sketch. Press the MMB to “pan” view. And SHIFT+RMB, to rotate. While Sketch is active, use Pad tool to extrude the object. Within pad dialog, enter 20mm Length. Use CTRL+SHIFT+RMB to zoom. Start new sketch. Now, select XZ plane. Now, change “draw style” to wireframe. Draw two lines, as shown. And add constraints, one by one. Select left vertex of the horizontal line. And simply assign vertical constraint. Enter 20mm for length. Then, select same vertex and vertical axis. And apply “fix to an object” constraint. Always pay attention to degrees of freedom. It will report if there’s an issue, or solved sketch. Next, select two vertices, as shown. And make them coincident. Then, add vertical distance constraint, and enter 6mm. Select horizontal line, and add constraint accordingly. Enter 25mm. Now, make sure you are using End points and Rim arc. Draw two arcs. Define end points, and then center/radius. For the smaller arc, add angle constraint, 35mm. Then radius, 8mm. Make two vertices, as shown, coincidence. When arc has constraints as in this sample, notice, how it’s more easier to control it. For the larger arc, make two vertices, as shown, perpendicular. Now, for the last two vertices, select them, and pay attention to degrees of freedom, when tangency is applied. We have fully constrained sketch. Next, while sketch is selected, apply Revolve. Within the dialog box, we can use default settings, but, we can use base z axis, as well, both share the same axis, in this case. Return to default shading. Select top face of the cylinder. And start new sketch. Change shading to wireframe. Select Line, and draw three of them, as shown. Now, select all three, and make them constructional. We’ll use them as guides to construct our sketch. Make first line symmetrical to the center. Select both vertices and center. And, apply symmetry constraint. Also, set vertical distance to 100mm. Apply symmetry on other two lines, the same way. Make them all equal, by selecting them, and apply equal constraint. Next define angle, between lines. First, select two of them, and apply angle constraint. Enter 60. Add circle, constrained to the center, and radius to 35mm. We’ll notice fully defined sketch, and ready to go to the next step. Add 6 more circles at each intersection. While adding circles, make sure that center, of each circle, is constrained onto construction lines. To one of the circles, add radius of 8mm. Then, select all of them. And apply equal constraint. Next, select each center, and make it constrained to the construction circle. When sketch is fully constrained, close the sketch. Return to default shading. Now, we want to use this sketch to remove some parts. We’ll use Pocket tool. And use Through all. Click Ok to complete the Pocket tool. Next, select bottom face. And start new sketch. Create Circle, coincident with the center, and radius 25mm. Again, while sketch is selected, use pocket, and create a hole inside. Enter 18mm. Next, select face inside. and start new sketch. This time add two circles. Smaller 8mm, and larger 13mm. And close the sketch. Using Pad tool, extrude the sketch 32mm. Start new sketch. Now use XZ_Plane, and click OK. Change shading to wireframe. Again, add circle, and with the mouse over vertical axis, make center constrained to axis. Add radius of 5mm. Add 6mm vertical distance, as well. Now close fully constrained sketch. Return visibility to default. Add Pocket. And if we use Through all now, we’ll see it goes only in one direction. To change that, check Symmetric to plane option. Hole will appear in opposite direction. For easier selection, change again shading to wireframe. And select all vertical side edges. Apply Fillet, and in the parameter selection box, we can see all edges previously selected. While tool is active, we can change shading mode. And visually, and easier, adjust radius. You can change the values with the mouse scroll. Enter 4mm, and confirm the Fillet. The reason for adding vertical fillets first, is to create on continuous line for top, and the bottom. Now select two line, one for the top, and one for the bottom. Fillet will recognize both lines as continuous, and cover the whole line. Enter 1.5mm. Select inner circle, as well. And enter 2mm. We can play with the appearance, to have a better preview. Also, within View menu, we could use Texture mapping. And use the image as Environmental map. Then we could have a better look of a shape. Use any image you may find interesting. Thanks for watching!

About Ralph Robinson

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3 thoughts on “Freecad tutorial – Knob – Product design #101

  1. I tend to use the "Part" workbench…but I think it's time to switch to the "Part Design" workbench…thanks for sharing!

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