Product structure tools, Constraints, Move toolbar

Creating an assembly requires use of tools that are specific to the Assembly design workbench. Creating bottom-up assembly or even the top-up assembly requires knowledge of these basic tools. These tools are present under Product Structure tools toolbar, Move toolbar and Constraints toolbar. Let's first study these tools and then we will move to creating an assembly. 

Product structure tools

Product structure tools toolbar has the tools for creating new part or product files from within the workbench environment which you may do in a top-down assembly process. It also has tools for bringing in the parts that have been already created for the purpose of assembly. In addition, it also has some other relevant tools.  Below you can see all the tools that are present in this toolbar. Let's see these tools one by one.

Product structure tools toolbar

Component - The option is used to add a representation of the Product document in the specification tree i.e. it does not create a file. Using this you will be able to add product representation without actually creating an assembly file. To this component you can create / add parts as you wish. To add the component, after you select the tool, you will need to specify the Product (in the specification tree) to which you wish to add component. We will not use this tool and it is of no use to us at this point.

Components, Parts, and Products icons illustrated in an assembly specification tree

Product - To create a new product file within the existing product, you can use this tool. You may use this tool in case of top-down assembly design where you wish to have a new sub-assembly in the existing product file. To use this, you would need to first select the tool i.e. Product, subsequently, need to select the product in the specification tree under which you wish to create the new assembly document.  

Part - This tool is used to create a new part file in the assembly design workbench. You may use this tool in the top-down assembly design workbench to create part file within the Product document of your choice. To create the part file, you would need to select the Part tool, and then the Product under which you wish to create the document.  

Existing component - The tool is used to call a part / product that you have already created, and add it to the specification tree. After selecting the tool, you would need to specify the Product in the specification tree, under which you wish to add the Part or Product. This tool is particularly use to add first part in the bottom-up assembly design workbench.

Existing component with positioning - The tool is used to add additional parts / products in the assembly design workbench after you have added first part / product using the Existing component tool. This tool is similar to the above tool, but additionally it lets you position and manipulate the part with respect the already added parts. So when you use this tool, a window opens up that let you select lines for aligning the part with respect to some reference as well as rotate the part as needed.

Replace component - If you work on Microsoft Windows, surely you would have renamed a file after creating it. Sometimes if we rename a product or part file that is referenced in an assembly document. In such a case the file will lose link due to the name change. You can re-link the file using Replace document tool. The tool can also be used to simply replace a component with another component. To do this, select the tool, followed by the part / product you wish to replace in the specification tree. This will open up the file dialogue box, which you can use to point to the file you want to add. 

Graph tree ordering - The tool can be used to reorder parts in a Product file in a sequence of your preference. To use this tool, a dialogue box is provided after you select the tool. Using the toolbox, you can move the parts / products up or down. 

Dialogue box - Graph tree reordering

A think to keep in mind is that the tool provides the dialogue box and only woks if you select the Product in the specification tree. Selecting a part will not open the dialogue box.

Generate numbering - If you have seen service manuals or AC, Car, Bike etc. You would have seen that parts are often numbered. This serves many purposes, like ensuring that total count of parts is provided, making communication easier etc. 

Dialogue box: Generate numbering

So, to generate this numbering, we can use this tool. The numbering that you generate here cannot be seen, and comes to use when we create the drawing of an assembly. We will see how this comes to use in the drafting workbench. 

Selective load - The tool is used in case you are working on very large assemblies that take a lot of computer's RAM and processing power. So, it becomes important that you load only or few parts that you need to work on, the rest need not be loaded. 

Selective load: Settings to be changed before reopening the assembly

To use this option however, the option Load referenced documents needs to be unselected in the settings. This will ensure that the next time you open any assembly, none of the parts / assemblies referenced load in the environment. 

Dialogue box - Selective load

To load the required product / parts, you can use the selective load tool, followed by selecting the Product / part in the specification tree. After the selection, when you press the button present beside the open depth level selector, it will show the part / product that will be loaded. To load the part / product press 'apply'.

Manage representations - The tool is used for CGR and model files management. It does not concern us as it is a relatively advanced topic and has no use in creating as assembly, so we will skip this at the moment. 

Define Multi instantiation -The tool can be used to call multiple part / products at once. To define this, you need to have at least one instance present already in the specification tree. 

Dialogue box: Define Multi instantiation

The locations at which these multiple instances are called can be defined using some of the same options that we used for creating pattern like Instances and Spacing, Spacing and Length, Length and Instances. Simultaneously direction in which these instances are created can be defined using axis or any element direction.

Fast multi instantiation - The parameters, method and number of instances defined above will be used directly if you use this tool. So, this tool can be used if you wish to create instances swiftly using previously defined parameters.

Move toolbar

We need to move the parts in space and get them into position where we can visualize them properly, so that constraints can be applied, and their degrees of freedom is arrested. So, the Move toolbar has tools that let us manipulate parts and assemblies in the environment.

Tools present in Move toolbar

Manipulation - The tool will open up a dialogue box, using which you can move the part as you desire. For example, you can choose movement in XY plane, YZ plane, or movement / rotation about an axis. 

Manipulation dialogue box

The dialogue box also provides the option to move parts / products with respect to constraints, to do this, select the option 'With respect to constraints'. This option will ensure that even if you select a manipulation option it works only if it is not restricted by the applied constraints.

Snap - Snap is an easy tool to align faces or edges of parts. To do this, select the tool and select the different edges of the parts that you wish to align or snap together. To use this command, you can either select lines, edges or faces of the different parts that you wish to snap together.

Smart move - It's a really fast way of moving the parts while simultaneously applying the relevant constraints. To use this, preselect the two parts between which you wish to apply constraints or move, then select the tool i.e. Smart move. 

Smart move dialogue box, you can apply constraints as per preference. Component selection can be switched using 'Next component' option

You can define the constraints preference list, and choose to apply the constraints as per your order of preference by selecting the option 'Create verified constraint first'. If you do not select the option, the constraints will be applied as the program sees fit.

Explode - Explode option can be used to create an exploded view of an assembly, which shows all parts, sub-assemblies etc. Such a view may come useful for people who need to assemble parts for manufacturing and can be used for defining sequence of parts to be used during assembly. 

Explode dialogue box.

The explode view is generally used after all constraints are applied. There are several options to choose from, like you can keep one of the part as fixed, so that it does not move during the explode command. You can also select the depth levels to which the explode is applied etc. Type will define if parts will move 2D, 3D or constrained in the explosion. The explode tool is only used after constraints are applied, since if you press OK without constraints, the position will change permanently. However, if you have applied the constraints you can bring the parts back to initial position simply by using the shortcut for update i.e. Ctrl + U. 

Stop manipulate on clash - The option can be activated and can be used with Manipulation tool. So when you manipulate parts with the option 'With respect to constraints' selected, you will find that parts will stop moving when they come in contact / clash with other parts. 

Using compass to move parts in assembly

Instead of using move toolbar, which is somewhat slow, you can use compass to move parts in space. To do this, simply select the base of the compass, move it and place onto the part which you wish to move as shown. The compass will turn green and now you can move the part directly using compass as shown. To freely rotate the part, you can use the top spherical part of the compass.

Using compass to move parts in assembly

To reset the compass and move to default position, grab it by the base again and leave it at the bottom right corner. It will automatically move to its default position. Instead of always moving the compass to the parts, you can instead right click on the base of compass and select the option "Snap automatically to selected objects", this will help to move parts more quickly in the assembly.

Constraints toolbar

The constraint toolbar is used to apply constraints between different parts and assemblies. This works very much like the constraints that we used in Sketcher workbench. So, you will find similar constraints like Coincidence, Angle, Offset etc. 

Constraints used in Assembly design

Applying constraints in an assembly is somewhat different however. In Sketcher, we did not use Fix constraint, however, as a rule, when the first part is brought in the assembly or the main part is created, it is fixed, by using the Fix component constraint. We will understand these constraints when we do the assembly. For the time being let's see the tools that are new.

Flexible / Rigid sub assembly - By default, when a sub-assembly i.e. a product is added using existing component or you create sub assembly, it is rigid. A rigid sub-assembly implies that position of the parts in the sub assembly, no matter how many times it is called, will be the same. However, using the Flexible / Rigid sub assembly tool you can change the sub assembly state to flexible. This ensures that relative part positions in the sub-assembly is stored at the product level and not at the sub-assembly level. Also, you will notice the icon change of the product in the specification tree. So, when you set the sub-assembly as flexible, you would be able to set the position of the parts independently in the different instances of the sub-assembly. We will see this in more detail when we do an assembly. 

Reuse pattern - This is a really fast way to assemble parts. If you used pattern while designing the part. It can become useful for assembling parts easily and you can use the same pattern for calling multiple instances of any one part that you may have assembled in one of the places. Also, you can use the constraints that you used for any one part assembled in position.