Designing a simple part

In this tutorial, we’re going to design a simple part consisting of a prism with a pocket in it. While the part itself isn’t particularly useful on its own, this should give a good overview on how to use Dune 3D.

The final part will look like this:


Open a new document

Start Dune 3D and create a new document.

Though not strictly required, you can turn off all workplanes but the XY one to reduce clutter by switching to the “References” group and turning them off.


When that’s done, remember to switch back to the “Sketch” group.


Use the “Draw contour” tool to create a sketch that looks like this:


Activate the tool either by

  1. The shortcut d s

  2. Opening the menu by pressing Space and searching for it

  3. The topmost button on the left side of the 3D viewport.

In the tool press a to draw an arc instead of a line. The tool automatically constrains almost-vertical/horizontal lines to be exactly that and creates coincident constraints when clicking on an entity. This and other behaviour can be configured with the shortcuts listed in the bar at the bottom of the 3D viewport.

Clicking on the starting point closes the path.

It’s best to start from the bottom-left or bottom-right corner so that the arc/line tangential constraints get created automatically. If these didn’t get created you can add them by selecting the arc and the line leading up to it and invoking the “Constrain parallel” tool.


In the workspace browser on the left side of the window, we should now see that our sketch has 4 degrees of freedom. Our goal now is to get this number to zero by adding constraints.

Arc center

Constrain the center of the arc to be on the origin of the workplane by selecting both points and invoking the “Constrain coincident” tool from the context menu.

To do so, first press Esc to clear the selection, then click on the arc’s center point, followed by the workplane origin. Order doesn’t matter. Finally, right-click on either of these points to open the context menu.


This should have removed two degrees of freedom. This added constraint is now also visible in your drawing as a violet symbol above the arc’s center point:



Select the bottom horizontal line and use the “Constrain horizontal distance” tool to set its width to 5mm.


To do so, right-click on it to invoke the constraining tool. Then drag the number that appears away from the line to make it easier to read. Double-click it to enter the distance.


We should now have one degree of freedom.


We want to constrain the total height of the sketch, but we first need to add a point that sits at the top of the arc.

To to so, use the “Draw point in workplane” tool to place point on the arc.

Same as all other tools, this one can be found in the menu by pressing Space and searching for it:


Use the “Constrain vertical” tool to constrain it to be directly above the arc’s center.

After this, we should still have one degree of freedom.


Select the point on the arc and one of the points from the bottom line and invoke the “Constrain vertical distance” tool to set the height to 6mm.

The end result should have zero degrees of freedom and look something like this:



With the 2D sketch being fully constrained, we can move on to make it 3D.

In the workspace browser in the left side of the window, click on the plus icon to add an extrusion group. You should now see a grey solid appearing. If you can’t see it’s sides rotate the view by dragging with the right mouse button. See Usage for how to navigate the 3D viewport.

You can change its height by dragging the lines on the top surface.

To set its height, right click on one of the vertical lines and select “Constrain distance”. If nothing appears, turn off the solid model by clicking on the cube next to “Body” in the left side of the window and drag the number so that it’s outside of the solid model. You may then re-enable the solid model and enter a distance value.


Create workplane

We now want to place a workplane at the center of the front face so that we can use it to create the sketch for the pocket.

First, create a new sketch from the plus icon in the workspace browser. Then, use the “Draw Line in 3D” tool to draw a line as shown below. We’ll use it later to center the workplane on the face. This is easier to do with the solid model off. Make sure to start and end the line from the two corner points so that the point-point constraints are created automatically. Watch tool bar the bottom of the window and the color of the points to make sure you got them.


Since we don’t need the line for anything other than placing the workplane, it can be a construction entity. To make it one, press g while drawing it or use “Set construction” from the context menu after the fact.

Next, add the workplane with the “Draw workplane” tool. Clicking on the middle of the line will automatically add the midpoint constraint so that the workplane sits at the center of the face. Again, watch the toolbar to make sure the constraint gets created as needed.


This has constrained the position of the workplane. We still need to constrain its rotation so that it’s in a plane with the face. For that, we’re going to use the “Constrain workplane normal” tool available from the context menu when selecting the newly-created workplane.


This tool requires you then click on the the line that corresponds to the workplane’s horizontal direction followed by a second line to define the plane. The workplane’s normal will then be perpendicular to both of the selected lines. If you get an error “please click on a line from a previous group”, this is because the reference lines can not lie in the current sketch and you need to have created a new sketch.

You should now have a workplane that looks like this. Make it this sketch’s active workplane by selecting “Set workplane” from its context menu.


Sketch pocket

To view the workplane face-on, double-click it or select “Align & center view to workplane” from its context menu.

With the new workplane in place, we can proceed with the sketch for the pocket. Start by drawing a hexagon with the “Draw regular polygon” tool. If the line drawing and polygon controls are grayed out, you need to select “Set Workplane” in the workplane’s context menu to make it the active workplane.


Constrain pocket sketch

To remove all degrees of freedom:

  • Constrain the construction circle’s diameter

  • Constrain the bottom line of the hexagon to be horizontal

  • Constrain the horizontal and vertical distance from the top-left point of the face

After these steps, the sketch should look like this:


Pocket extrusion

Create new extrusion, change its operation to difference and drag its end inwards so it looks somewhat like this:


We want the pocket to end 1 mm before the beginning of the semi-circle of the outer part. For this, we first need to draw a construction line so that we have something that defines the plane. Again, use the “Draw Line in 3D” tool for this:


Then, select the newly-created line, one of the other outer lines and a point at the tip of the extrusion to invoke the constrain distance tool and enter the distance.



As the last step, we want to add the chamfer on the top surface. For this, add a new Chamfer group and click on select edges in the group tab. In the select edges tool, select the edges as shown below and right-click to confirm the selection.


The chamfer group automatically applies the chamfer to tangent edges.


That’s it

The part is now done an can be exported as an STL for 3D printing.