Creating an assemblyДмитрий Зиновьев
An assembly is a set of interdependent components. Any assembly can consist of parts, other simpler assemblies, standard components and various elements.
Let’s review the major functions for creating assemblies.
Lets create an assembly. Click New and choose an assemble file Standard.iam.
Rename our assembly to Bracket and save it.
Our assembly will consist of parts, but first we have to create these parts. So, create a part.
In the sketch, draw a rectangle 200 by 500 mm with starting point on the origin. Select Rectangle, specify the start point, enter 200 on the keyboard, then press Tab, 500 and press Enter. Finish sketch.
Select the Extrude operation. Specify the distance as 8 mm. Click OK, and rename the part to Rack.
Open Properties and select the material Steel. Apply. Next, select the texture Blue Wall Pain Glossy. Save the part.
Let’s create one more part. In the sketch, draw a rectangle 200 by 200 millimeters with the starting point on the origin. Finish sketch and choose the Extrude operation, enter 6 millimeters.
After this select the Chamfer operation and make a chamfer on one of the faces, equal to 180 millimeters.
Rename the part to Rib, open it’s Properties and specify the material Steel. Apply and close.
For this part, we choose the texture Green polished. Save this part.
All the created parts and the assemble itself are displayed in the bottom part of the window as tabs.
Let’s open our assembly. In the menu Assemble, use Place to insert a component into the assembly.
Click Place and you will see the folder of the current project. Select the part Rack and click Open. One part immediately appeared on the assembly. We can create this position for several more copies of the part or press Escape (Esc).
In the browser area you should now see the inserted part with the clip icon. This means that the position of the current part is fixed. We can’t move it. If we right click on the name of the part, we will see the flag Grounded.
Let us insert one more part in the assembly. Select the Rib file, insert one part and press Escape (Esc).
As we can see, the position of this detail is not grounded.
It has six degrees of freedom, and we can both rotate and move it. You can move it by clicking and holding the left mouse button on the selected part. The rotation is done through the corresponding function Free rotation.
In order to determine the position of the parts’ relatively to each other, we use constraints.
Lets review assembly constraints.
They differ by type: alignment, angle, tangent, and insert. For any constraint there are two options: Mate and Flush.
We choose the Mate option and first specify the face of the Rack, than the face of the Rib.
If we check the point With preview, we can immediately see how these parts are connected. We can specify the offset between the parts. In our case we leave the offset equal to zero and click Apply.
Lets create one more place constraint, but this time choose Flush. Choose the desired faces on the Rack and the Rib and press Apply.
The Rib part has one more degree of freedom left. Apply the place constraint, choose Flush.
Click on the side of the Rib and front face of the Rack.
Specify the offset as 246.
Now the position of the Rib is completely fixed.
Save the assembly.