Working with CAD platforms is an engineering area in which the ideas for new concepts and imagination are unlimited. It is impossible to create fixed standards about how to design new products, which design features to be used and how to strictly organize the model tree structure. This is entirely up to the mechanical designer. Each CAD user has his own vision and ideas how to use a certain software for his design work. But however in order to work efficiently with any CAD you still have to learn how to apply design strategies. Improved design strategies can result in new design versions for similar or the same product and if applied correctly they can also save precious time, for example only changing a specific area on your product without changing the main geometry.

In this post I am going to show you how to apply 2 different design strategies working with Generative Shape Design creating surfaces and then adding volume with Part Design workbenches with CATIA V5. The part I design here is a bottle opener having different designs in the middle area but keeps the size and the rest of the geometry the same.



Create a new part.


Create and rename the model Tree structure as shown.


Start creating the wireframes. The first being the main half-profile as a planar sketch using the profile icon. So pick a plan – for example XY- and draw the necessary lines and circles, constrain them as shown then exit the sketch.


On this main sketch, add 4 planes normal to curve, coincident with the points on the line as shown:


On the each of these 4 planes, draw a spline made of 3 points with “Tangency” option activated on both ends. For the 3rd sketch create 2 such splines and make them coincident in the upper point and constrained as shown:


The design of this bottle opener is made of 3 main zones namely: the Handle area, the Middle area and the Opener area. Therefore, the design strategy applied here is to define these 3 surfaces area by splitting the main profile accordingly. Create the surfaces in each area then join them together. First you must create surface for the Opener area, then do the Handel Surface and the last one would be the Middle surface.

Create the 1st Split for the Opener area by keeping the Optional parameter “Keep both sides” activated. Then do the same for the 2nd Split at the bottom of Handle area.


Having the main sketch profile splited, the next design step is to sweep the surface profile along the defined cuts. Therefore click on the Sweep “icon” and create the reference surfaces as shown:


To design the Middle area, first you need some construction elements. For that create a plane using the inner edge of the Opener area as reference then on this plane draw a sketch using the “Three point arc” making its center coincident with the symmetry plane and after making one end point also coincident and tangent with the inner edge, the other point must be symmetrically constrained as well.


To create the rest of the Handle and partially the Middle area, create the next 2 surfaces using the “Multi-Section Surface” feature with the parameters as shown below:

STEP 10.

At this stage the half-side of the bottle opener is almost done. You can Join all the surfaces created so far.

STEP 11.

It can be very possible that this newly created surface is not really entirely all on the same side of the symmetry plane therefore if that happens, cut the unnecessary side by clicking the Split icon in the “Operations” toolbar.

STEP 12.

Now the half-side is correctly cut, so it can be mirrored with the “Symmetry” feature versus the symmetry plane.

STEP 13.

Keep working on the Middle area and split the Sketch nr. 3 as defined at Step 5. by its middle point, keeping the optional parameter “Keep both side” activated.

STEP 14.

Connect the inner surfaces of the Opener, with a Surface Sweep along the Sketch you´ve created at Step 8

STEP 15.

Create a surface Fill on the gap between the 3 areas (Handle+Middle+Opener). Then join everything together.

STEP 16.

Front side surface of the part is now ready. But to add some volume and make your part design fully defined, you must define the back side as well. This is very simple to do.

Select all the edges of the Front-side surface and create a surface Fill feature in order to close the back side.

STEP 17.

To create the opening on backside you can use as boundary the inner edge of the front surface and create an extruded surface with it.

STEP 18.

Cut the Backside surface with the extruded surface. Then cut again the remaining extruded surface with the resulted back surface.

STEP 19.

Join all the visible surfaces

STEP 20.

To add volume , first of all make sure the PartBody (or as renamed Opener_Body) in Model tree is the “In Work Object” and click in Surface-Based Features toolbar click on “Close surface” icon and select the last Join feature.

After that you can do one more dress-up feature by shelling the backside at say 1mm thickness.

STEP 21.

To make it look nicer you can change the color as well.

The design version A is finished an looks like this:



For the second design version, which is only different in the Middle area, to reduce the design work you can save the first design version with a new name and only modify the design in the middle area. So assuming you have the design A still open, in the File menu, click on “Save as…” and rename the file as new version.


Keep the design work the same like for version A until step 8 (included) and continue from here by applying a Split done with the symmetry plane on the sketch that represents the lower inner edge of the Opening.

The data you need to create the version B looks like this:


On the Symmetry plane draw a sketch made of 2 separate splines of 3 points with Tangency activated at their end points and then make these splines coincident as shown. This point will remain visible when you exit the sketch. Put the rest of constraints and exit the Sketcher workbench.


The wireframe result of the previous sketch is a curve with a point in the middle. Project that point on the main profile line and create a plane normal to the line profile in that projection.


On the previously created plane sketch a profile using the Spline feature made of 3 points with tangency option activated at both end points. Make the upper point perpendicular and coincident with the symmetry plane.

Then on the symmetry plane draw a straight line coincident and tangent with in the middle point of sketch created at Step 3 (design version B)


Create a plane rotated with 90° angle versus the symmetry plane around the last straight line. And on this plane sketch another straight line coincident in the same middle point and at 35° angle versus the symmetry plane.


Now in GSD workbench connect the 2 upper points with a 3D Spline with a Tension parameter of value 1 at its both end points.

As construction element helpful to generate smooth surface extrusion, just sketch a vertical line coincident at one end with the end point of the split previously done at STEP 6.


Use the sketched profile from Step 3 and create an extrude feature of approx. 5mm length, then use the edge in the symmetry plane of this extrude to create a multi-section surface that will close the lower side if the middle area.


Continue creating the second Multi-Section surface that will close the Middle area sidewise. Then similarly create the 3rd one to close the upper side of the Middle area.

STEP 10.

Hide all the surfaces on the left side of the symmetry plane and join all the other surfaces on the right.

STEP 11.

Mirror the Join surface on the Symmetry plane, join again the result with the right side and from here just repeat the remaining steps starting from STEP 16 as shown at the first design version.

Design version B is ready and it looks like this:

The Bottle opener is now finished . The same product done with 2 design strategies.

This exercise is also available as video version on my YouTube Channel as shown below:

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