This exercise was carried out with version 27.0 (Vertex 2021).
Table of Contents
In this exercise you will learn to
How to a new part (local) is created in the assembly.
How to create a part from lines and faces.
How to give color and transparency for a part to make it easy to use as a jig.
The actual sheet metal parts are modeled in the next exercise.
Functions to be used:
Creating a new part in the assembly.
New Sketch > Face, Parallel, 3D Skecth
Sketching:
Operation: Guide Curve
Faces > Add Face
To volume (Create a part form faces. Add a missing faces.)
Add Round/Bevel > Single Edge Round
Rendering > Change Material
Rendering > Change Transparency.
Main stages
Sketch the inside shape of the jig using the Guide curves.
Use these guide curves to add faces.
Create a part (volume) of the faces.
Add roundings used when creating sheet metal parst with the Tangential offset function.
Create a new Assembly
File > New > Assembly.
Enter the label (which is also the name of the model and by default will be the name of the drawing).
Enter the archive information by clickingArc.Data.
Select the project where the model will be saved.
OK.
Create a local part
Right-click function: New.
Click: Part.
Enter the label of the part.
Select: Local. "Local" means that the part is not made its own file, it is only visible in the assembly.
Create a Guide curve for bottom
New Sketch > To horizontal (XY) plane.
Sketch the shape
Sketch a rectangle. The function: Two point rectangle.
Click to the first point from the origo.
Enter the dimensions: 200,150 and press the enter key.
The program draws a rectangle with size 400 * 300.
If you want the jig to vary in size, edit the dimensions and add a formula to them
Operation
Guode Curve.
Create a Guide curve for top
Restore the Horizontal (XY) Plane if it is hidden.
Click the Plane.
Right-click function: Restore.
Click the To horizontal (XY) plane.
Right-click function: New Sketch > To parallel.
Enter value 400 and formula HEIGHT
Sketch the shape
Skecth a rectangle in an oblique position.
Skecth construction lines, between the middle point of lines.
Add the Conincident constraints separately for each construction line and ogigo.
Add the Distance constrains.
400 and formula: LENGTH.
300 and formula: HEIGHT.
Add the Angle constrain
25.
Operation
Guode Curve.
Sketch a 3D guide curve
Right-click function: New Sketch > 3D Skecth.
Add eight lines as shown in the figure.
Make sure the cursor catches the endpoints of the lines and not the lines.
OK. (Exits sketch mode and makes guide curves).
Add surfaces
Surfaces have to be added for each Face (10 pcs) separately.
Click three adjacent lines. (Remember the Ctrl key).
Right-click function: Faces > Add New.
If necessary, change the direction so that the arrow points outwards from the "part".
Use the option for the following faces: Stitch surfaces.
This option to keep the faces to be joined parallel (= outwards from the "part"), so the part (volume) can be easily formed later.
Create a part (volume)
The edges between the surfaces cannot be rounded, so surfaces must first be made a volume.
The surfaces in the model should form a enclosed space, but this is not an absolute requirement. It is allowed for someone or some faces to be missing.
Right-click function: To Volume.
Click a reference face (Any of these faces are valid).
OK.
Note: If you have modeled (all needed) the surfaces so that they delimit the enclosed space from space, the program may not introduce the right-click function: To Volume. In this case, you can create rounds directly to the model.
Create roundings
Click the four lines shown in the figure. (Remember Ctrlkey).
Right-click function: Add Round/Bevel > Single Edge Round.
Enter the value for the bending radius of the plate, eg: 2.
