6.3.2 Subassembly - Further Components

After the 11er_Balken has been installed and clearly positioned, the other components will be installed. They are NOT positioned absolutely, but referenced on the 11er_Balken. 

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In the toolbar Assemblies choose Add and search for the part steckverbinder_stange as described.

Confirm with OK.

The Steckverbinder_Stange is not to be positioned absolutely, but referenced on the 11er_Balken. To do this, select the menu option By Constraints under Positioning. Confirm with OK. (Figure "Add Component Steckverbinder_Stange")

 

The Assembly Constraints and Component Preview windows appear. (Figure "Assembly Contraints") und (Figure "Component Preview")

 

If you check the "Preview Component in Main Window" box in the Assembly Constraints window, you can observe the orientation of the part while setting the positioning conditions.

 

Under Type you can now select the connection conditions required for the assembly. The following relationship conditions are available to you:

Button	Name	Function
	Touch Align	Touch: Surfaces are joined in opposite directions. Align: Surfaces are joined in the same directions. Infer Center/Axis: Centred insertion of cylindrical elements, e. g. shaft into bore. When selecting a cylindrical or conical surface, the center or centre axis is selected here.
	Align/Lock	This is used to align the axes of cylindrical elements. At the same time, the degree of freedom of rotation of both elements is fixed to each other. Advantageous e. g. for inserting screws.
	Bond	This "welds" two elements so that they appear as rigid bodies.
	Angle	Connection through an angle.
	Parallel	Parallel arrangement of e. g. datum planes, surfaces etc.
	Center	Centers one or two elements between a pair of elements.
	Concentric	Concentric arrangement of two bodies. Note that the selected circles are on the same level.
	Distance	Position elements with a defined offset to each other.
	Perpendicular	Position elements perpendicular to each other.
	Fit	Adds bodies with the same radius into each other. If the radii become unequal, the connection becomes invalid.
	Fix	Provides the possibility to fix a body on the current position.

Make sure that you use the functions according to the application. Especially the functions "Bond" and "Fix" should be used wisely. "Bond" is only used if the parts are actually to be welded. This means that they should be inextricably linked. However, it is primarily intended to make plug-in and bolted connections. The "Fix" function, on the other hand, is only intended for one part that serves as a reference element for all subsequent parts.

 

Difference between Touch Align and Concentric:
Although not immediately obvious, the two functions differ considerably. With both functions, cylinders can be positioned on the same central axis. The difference is that with Concentric, the selected cylinder edges are placed firmly on a plane and an error message appears when the edges are moved (Figure "Difference "Touch Align" (left) and "Concentric" (right)"). In order to arrange two cylinders on the same axis but with a distance to each other, we recommend the following procedure: The cylinder axes are to be placed on top of each other with Touch Align and the selection Align under Orientation . You can then use the "Distance" function to define the relative displacement.

You can view, edit and delete all already set links in the Assembly Navigator under "Constraints". In assemblies with many parts it can be problematic to select a certain edge, surface, plane etc.

 

With the filter function you can select specific elements, since all other types are no longer selectable. The filter function can be found in the upper left corner of the start menu. (Figure "Filter")

Furthermore, there is also the possibility to move parts by means of the Move function based on their still open degrees of freedom. To do this, you must leave the window in which you assign the assembly constraints and right-click on the desired part. Now select Move. Moving works in the same way as moving the WCS. You have several options for terminating the function:

• OK: The menu closes and the part remains in the position you have moved it to.
• Apply: The part also stays in the new position, but the menu remains open and the part is deselected so that a new part can be selected and moved.
• Cancel: The menu is closed and the part is reset to its original position, the movement is not carried out.

You can also right-click on the part in the Part Navigator or in the model to select Show Degrees of Freedom.  The still open degrees of freedom of movement are now displayed as red arrows. This information is used to change the position of the part or to set missing assembly constraints. After you have set an assembly constraint, press F5 to update the open degrees of freedom view and remove the red arrows.

 

To reference steckverbinder_stange to the 11er_Balken, you can use the Infer Center/Axis linking condition. Select the surface of the cylindrical end of the Steckverbinder_Stange and then select the surface of the hole in the 11er_Balken. To restrict the remaining degrees of freedom (rotation around the center axis and translation along the center axis), it is advisable to use the connection conditions Touch and Parallel.
If you have closed the Assembly Constraints window too early and the part is not fully aligned, you can add more relationship conditions later. To do this, click on the part to be referenced with the RMB. In the context menu that now opens, click on Assembly Constraints and proceed as usual with alignment.

Now install the remaining parts and the subassembly ubg_sensor_tast with the now known functions. Please refer to the pictures:

• Steckverbinder (2x) and Steckverbinder_Stange (2x) Figure "Zwischenstand 1"
• Stangen_Querverbinder (2x) and 5er_Stange Figure "Zwischenstand 2"
• Parallelsteckverbindung and Steckverbinder_lang Figure "Zwischenstand 3"
• Parallelsteckverbindung and UBG_Sensor_tast Figure "UBG_Sensor_hinten_gesamt".

Note:

If you require reference objects (help geometries), it makes sense to create them in the individual parts. Therefore, when assembling an assembly, you should consider where axes or planes are still needed in the corresponding component. With "Make Work Part" (select via the Assembly Navigator and then press the right mouse button) you can then insert datum geometries in the part. This temporarily changes you to the individual part processing.