Part Creation Using XDesign

   By Haley Huffman on April 26, 2023

3DEXPERIENCE brings all your engineering software and project needs all to one platform. In our TriMech “It’s Time to Collaborate” webinar series, the TriMech team uses 3DEXPERIENCE to take an alarm clock project through a typical design cycle. Below are some of the parts of the assembly using XDesign not covered in the first design webinar and how to design them will be shown step by step.

The first piece to be created will be the metal clock housing. A two-dimensional sketch will be created, revolved three hundred and sixty degrees, and then a series of holes and slots will be cut into the housing. First create a sketch on the yz plane that will become the profile of the revolve as shown below. In addition to the profile sketch in the shape below, sketch fillets at each vertex are added at a value of 0.05mm.

sketch fillets at each vertex are added at a value of 0.05mm

In addition to the above profile sketch, an axis piercing the xy plane needs to be created.  Once done, choose the revolve feature under the features tab. The dialog box as shown below will pop up, choose a thin feature which allows open sketches to used as a profile sketch, choose full revolve from the drop down under direction, and set the thickness to 0.05mm.

set the sketch thickness to 0.05mm

Once the revolve is created, a reference plane should be created that is parallel to the yz plane just is tangent to the revolved surface. This can be done using references or offsetting the yz plane by 3mm. Once the reference plane is created, two sketches will be created to make the necessary slot/hole cuts. The first sketch will be the centerline slot, which will be located 3mm from the top of the metal housing, 0.7mm in height, and 0.5mm wide. Once the sketch is created, choose an extrude cut under features, in the dialog box choose up to geometry under direction one, since it only goes through one side of the housing, and under geometry choose the inside face of the housing.  In the second sketch, create two symmetric circles on the same reference plane as the previous, that are 6mm apart, and 0.045mm in diameter. Once this second sketch is created, choose an extrude cut for both circles, and under direction one choose through both ways.

create the reference plane

extrude cut for both circles

To create this part a series of two dimensional sketches and extrusions will be created.  The first sketch is a trapezoid, an overlapping circle and tangent arcs as endcaps on either base of the trapezoids.

tangent arcs as endcaps on either base of the trapezoids

This is then extruded 0.1mm. Another sketch can then be created on the circle face, where the sketch is of the same 0.6mm diameter circle centered on the origin that is then extruded up(blind) 0.05mm. This geometry is then filleted at 0.05mm with tangent propagation on so that it captures the entire face. The final step is created another circle sketch on the bottom face of the geometry that is a diameter of 0.1mm and blindly extruded 0.4mm.

circle sketch on the bottom face of the geometry

The 3DEXPERIENCE platform makes design and collaboration simple. Above individual part creation using XDesign was covered and in the design webinar multifaceted parts and subassembly creation will be demonstrated using the platform.

Related Products
3DEXPERIENCE Apps

Browse the TriMech web store for 3DEXPERIENCE Roles and Apps to design, analyze and manufacture your products on the cloud.

Haley Huffman

Related Content

Graco Hand Tool

Graco: Nylon 3D Printed Pressure Check Hand Tool

Graco Inc. supplies technology and expertise for the management of fluids and coatings in both…

Learn More...
P3 & CLIP

What are the differences between P3 and CLIP 3D printing technology?

P3 vs CLIP As 3D printing continues to evolve and revolutionize the manufacturing space, the…

Learn More...

Creating Lofts in SOLIDWORKS

Part modeling in SOLIDWORKS can go far beyond what our imagination is able to create….

Learn More...