When I come across a new product with an interesting design, I often challenge myself to think through how I would model it in xDesign. Recently, my wife mentioned that Owala water bottles have “the best design.” Given that she uses a water bottle constantly, her comment immediately caught my attention.

The product combines a vacuum-sealed metal container with a thoughtfully engineered lid. The lid features an overmolded rubber exterior, a dual-function spout that supports both pouring and sipping through a straw, and a spring-loaded hinged cap that seals securely to prevent leaks. Additionally, the integrated handle follows the curvature of the lid and shares the same hinge axis as the cap, allowing it to remain compact when folded down while still being comfortable to hold when raised.

To better understand the design, I deconstructed the product and analyzed how it could be modeled. It quickly became clear that the lid was the most complex component. The cap and handle could then be built in context once the lid geometry was established. One of the most interesting aspects of this design is that it requires a surface modeling approach to accurately capture its form.

Surface Modeling Approach

Lid:

1. I started by revolving a domed surface that followed the overall size and shape of the cover.
2. Next, I sketched a mound-like profile that followed the curved bump in the middle and low points on the front and back.
3. Then used the Surface Trim tool to trim away exterior surfaces.
4. This defined the outer surfaces for the cover. At this point it is still an open surface model as indicated by the blue surface edges.

1. The next step was to remove the interior of the cover. I extruded a pill-shaped profile vertically through dome shape.
2. Used the Trim Surface feature once again to remove the inside-top face of the curved top surface and the top faces of the extruded surface that extended above the dome.
3. To create the top surface of the cover where the cap sits, I extruded another profile horizontally through the dome. This time I extruded it from the midplane making sure enough of the surface extended around the outside of the dome on all 4 sides.
4. Then trimmed the outside of the interior top surface using the vertical extruded surface from step 1 above.

1. Now a need to close up the surface model so I used the Fill Surface command to create a circular patch on the bottom. Then, I used the Knit command and selected all 5 surface bodies and merged them with Make Solid option check on. Now all edges will be black indicating solid geometry.
2. I shelled cover which worked nicely except there were 2 small voids that inside the 2 'ears' that stick up towards the highest points on the model as seen in image 3.

3. Image 3 shows a section view cutting through the middle of the ears so that you can see the small voids. I used the Delete Face command that has Replace option.

   
4. Image 4 shows the section view again after the Delete Face feature.

1. Next, I needed to work on the spout. I sketched a circle on the XY Plane at the bottom of the cover and created an Extrude feature. The xDesign Extrude feature is full of great options. Since the spout is on the top outside of the cover, normally, I would create another reference plane above the cover but it is faster to use the From Offset Start Condition under Advanced in the Extrude command. After selecting the sketch, I can simply drag the extrude body up using the ball manipulator. Then, I used the Up To Geometry end condition for Direction 1 to have the cylindrical extrude terminate at the curved top surface highlighted in pink above. Before leaving the Extrude command, I selected the New option instead of the default Add option at the top of the dialog.  This creates a new body for the cylinder instead of merging it with the existing solid geometry. I needed the cylinder to be a separate body to achieve the lip cut-away in the next step.
2. The spout has a curved cut-away on the front of the cylinder for your bottom lip to use while drinking. I sketched an arc on the ZX Plane, leaving the endpoints of the arc outside of the cylinder.  I sketched a centerline that was to the right of the center line for the cylinder to make a wide elliptical cut-away. I created a Revolved surface from the midplane at 150deg. I then selected the Cut option and unselected the Auto Merge option that allowed me to only select the cylinder for the cut to merge with. The cut would have failed if it tried to merge with the main body for the domed cover.
3. Since they are 2 bodies, I used the Combine command to merge the 2 bodies together.
4. Next, i sketched a circle on top of the cylinder and did a Extrude Cut through all.

1. The large cylinder will be used for pouring, but there is a small tube that runs along the inside front of the cylinder used for sipping through a straw. This curvy tube can be created using the Loft command. I started by offsetting a new reference plane from the XY plane near the bottom and sketched 2 concentric circles for the bottom of the sip tube. Then I drew 2 concentric ellipses on the top front of the cylinder. I connected the center points by sketching a vertical S-shaped spline. I used the spline handles for each endpoint and made them vertical. This vertical spline will be the Spine Curve used in the Loft.
2. I created a solid Loft using the outer ellipse sketch from the top and the outer circle sketch from the bottom, then selected the spline as the spine curve. Then created a second Lofted Cut using the inside sketches from the top ellipse and bottom circle and again used the spline for the Spine Curve. It worked very nicely. The only issue is that the loft feature poked through the front of the cylinder inside the lip cutout slightly.  So, I used Delete Face with Replace option to fix that quickly.
3. I blinded the edges of the loft inside the spout by creating to large fillets on the 2 edges where the loft intersected with the inside of the tube/cylinder.
4. To finish the spout, I used a curve sketch to cut through the top of the cylinder.

1. I needed to fill in the area between the sip tube and inside walls of the cover.  There is a small block of material in there indicated by the red arrow. I extruded a rectangular block upwards filling in the gap and using the Through Next end condition which merged nicely as intended.
2. I added some draft to the inside faces of the ears and the inside surface wrapping around the top of the cover.
3. Then I extruded a cut from the outside front of the cover while cutting through the front of the dome and partially cutting into the cylindrical spout.
4. Lastly, I created a Split Body feature to make the red band color break as shown.  I then colored all of the faces around the spout and the rectangular cut for the button - which I worked on next.

Button:

1. It was very easy for me to create the button in an xDesign component as a separate body. That way I can model in context of the cover part and reference the button area I cut out. The best way to do this is to create a new Folder called an Ordered Geometrical Set (OGS). Each Set can have geometry that does not merge with geometry from other sets such as the default set named Design Features. To create a new set, RMB on the 3DShape at the top of your tree under the component and choose Insert Ordered Geometrical Set. Once it has been added to the tree, slow double click on it and rename it Button. It should be active and the name should be bold in the tree. The rollback bar is always shown in the active set once you have some features in there.  Double click on the sets in the tree to activate them. Careful to not build geometry in the wrongs set so pay attention to the active one.
2. Next I sketched a rectangle on the bottom surface of the cutout in the cover. The rectangle was slightly narrower than the zone to leave some clearance.  The front of the button extends in front of the cover front surface a bit.  I created an Extrude using the rectangle sketch and offset the start condition to be the same clearance as the sides. Then the extruded height should also leave clearance. Once you hit OK, it will be a new body in the Button Set.
3. Next I sketched a profile on the YZ Plane that defines a revolved cut that creates the notch that holds the Cap component closed and then a chamfer on the front of the button. The Revolve Axis in the same as the axis for the dome cover. Then I sketch another profile (not shown) on the horizontal bottom face of the notch area and Extrude Cut a circular profile that is concentric to and slightly larger than the spout cylinder.
4. Lastly, the bottom face of the notch area (used for the last sketch) it too flat and should follow the curve on the ridge on the cover - the area that got cut away. Select the back face of the button cutout in the cover zooming into one of the clearance areas and start a sketch. Draw a curve to match the ridge, then extrude a surface out pas the button slightly.  Then use the Delete Face command again and replace the flat surface with the new curved one.
   The dimple on the front is very easy to do. You start by creating a Spere Primitive. Once the command starts you will see a temporary preview of the sphere stuck to your cursor. You move the cursor over the front face of the button, then click on it. As soon as you click, a button will appear next to the face called Center On, Click the button to center the sphere to the face. Even though it is sitting tangent to the face, choose OK on the command. Now start he scale command and select the sphere. Choose Non Uniform Scaling option and enter .5 in the Z-Scale-Factor input. Choose OK. Next start the move body command and move 1.25mm in the negative X direction. Lastly, choose the Combine command and remove the squashed sphere body from the switch body.

Cap:

1. The workflow to create the flip cap is similar tot he cover but simpler. Start by creating a new Set like we did for the button and name it Cap and make sure it is active. To sketch the side profile for the cap we need to see the curvature of the top surface on the cover. You can either view Hidden Lines using the View Modes command from the View Tab on the Action Bar or create a section view. Select the ZX Plane and create a sketch. Sketch the wedge-like shape with the bottom curve following the curvature of the tope surface in the cover. Then do midplane Extrude as a closed solid this time instead of surface. The hinge point will be determined from the arc on the right of the sketch. I will not detail all of the features for the remaining components and just give my overall design intent strategy.
2. Now create a 2nd sketch on the on the XY plane, making sure to be working in the new Cap Set. Sketch rectangular shape shown with full round at the front of the cover as shown above.  Extrude this as a New solid body. Make sure to choose New instead of Add.
3. You can see how the 2 bodies overlap in image 3 above. Start the Combine command and choose Common, then select the 2 bodies. You will be left with the intersecting body which represents the overall shape for the cap.
4. The last image above shows the complete cap component that is shelled, has 2 small pins for the hinge and a tab on the front edge to interact with the button to keep the cap in the closed position. I will not go through all of the features but you can investigate from the included model.  Since the hinge is defined, you can create the cuts in the Cover part for the hinge too. To do this, activate the Design Feature Set which contains the geometry for the cover. Start a sketch on the ZX Plane and select one of the edges at the end of one of the pins on the side of the Cap and Convert Entities. Create an Extrude Cut from the midplane and have it intersect with the 2 ears on the cover.  Since we are creating the cut in the Design Features Set, the Cap geometry is not cut but the cut references the size and location of the pins.

Handle:

1. I used a similar technique to model the Handle as I did with the Cap. The handle shares the same curvature as the cap and I wanted the handle curvature to reference the cap should it change later. Start by activating the Cap Set and rolling the tree back to Combine feature where the 2 bodies were merged into one using the Common mode. Create a Surface Offset feature in the rollback state within the Cap Set, select the 3 faces going around the front and sides of the cap and enter 5mm offset value.  Hit OK. Then drag the rollback bar to the end of the cap Set again.  You should see this new surface covering your cap, RMB on the new surface and choose Make Body. This will open a dialog, choose  New Ordered Geometrical Set and name it Handle. Hit OK. You should now have a new Set named Handle with a single feature named Offset, that is a linked surface body referencing the Offset in the Cap set.  You should now Hide the original offset feature from the Cap set.
2. Using a similar workflow as you did with the cap, unhide the Cover in the Design Features set and the button set. View hidden lines. Create a Surface Extend and select the 3 edges along the bottom of the surface and extend down by 10mm. Next, create a sketch on the ZY Plane. While viewing the side of the model like shown above, convert entities on the arc around the hinge so the handle matches the cap hinge. Then sketch some tangent arcs off of the hinge arc similar to what you see above.  The bottom of the profile should follow the same curvature as the top of the cover but extend out in front of the cover near the button. As you can see in the photos from top of this page, the handle extends over the button about half way.  This is another nice design feature because this will prevent the button from being pressed accidentally which would release the cap and have fluid leak out. Sketch the arc along the top of the handle and then close the profile with a straight line on the far left. Exit the sketch.
3. Now, create a surface extrude from the midplane and make sure the width of the extrude extends completely outside of the other surface. Create a Surface Trim between these 2 surfaces and keep the intersecting part in the middle. Use the Make Solid option.
4. Now you have the basic shape for the handle.  Create a Shell and select all of the faces around he top, bottom and the hinge as shown above.  I shelled it to 4mm, which will leave 1mm clearance around the cap. You can create hinge pins on the outer faces that match up with the holes in the ears on the cover.  Then create some hinge holes on the inside faces to match up with the pins on the cap.

Final Thoughts:

This exercise highlights the importance of surface modeling when working with complex consumer product geometries. By breaking the design down into manageable components and leveraging in-context modeling, it becomes possible to replicate intricate forms while maintaining parametric control.

The Owala bottle is a great example of how thoughtful industrial design integrates functionality, ergonomics, and compact packaging—making it both a compelling product and an excellent modeling challenge.