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SolidWorks Tech Tips – Assemblies


Locking and Breaking Assembly References

When working with external references in SolidWorks, it is extremely important that users understand the differences between Lock All and Break All. These functions, added in SolidWorks 2000, are for managing the associativity of features that are related to other part files or built in-context in an assembly. The functions are accessed by opening a part file that has external references. Place your cursor over the top-most icon of the FeatureManager, right-mouse click, and select “List External Refs“. At the bottom of the External References dialog are three buttons: Break All, Lock All, and Unlock All.

The Lock All and Unlock All buttons are very useful. Imagine that you are building two parts that fit closely together, such as the two leaves of a door hinge. Top-Down design techniques will allow one leaf to automatically update when you make changes to the other side. However, if you wanted to animate the hinge, and do motion of collision studies, this could cause difficulty — each time you dragged one hinge leaf into a new position, it could update the other hinge’s shape. So there are times when you want to temporarily prevent the top-down update process. Lock All does that. External references that are locked do not update with changes to the referenced file. Unlock All, of course, returns the model to normal updating.

Break All functions exactly the same as Lock All with the important difference that there is no Unbreak All button! This button is offered as the lazy man’s way of removing external file references. It is tempting to use this, instead of manually editing each sketch and top-down feature, to replace the external relationships with internal ones. However, at sites where large-scale product design is done collaboratively over the network, and where parts that have been subjected to the Break All command are used, CAPINC engineers have seen this feature can lead to corruption issues which usually result in the inability to open the top-level assembly file at all. It is CAPINC’s recommendation that users do not use the Break All button. Not ever. Never.

Viewing the Assembly Mates for a Particular Component

SolidWorks provides you with several ways to view which mates are associated to a component.

The most general way is to place your cursor over the top icon in the assembly FeatureManager, and right-mouse-click. Choose the option Tree Display – View Mates and Dependencies. This will place the FeatureManager in a mode where all the mates are grouped beneath their components. To return to the default display mode, right-click again at the top icon, and select Tree Display – View Features.

SolidWorks 2000 added a new assembly function to make mate searches even more convenient. Right-click over any component, and select View Mates. This invokes a split-screen display of the FeatureManager, and fills the lower half with the list of mates affecting that component. Starting with SolidWorks 2007, this command also shows callouts in the graphics window to illustrate the associated mates.

SolidWorks 2004 added folders on the FeatureManager for the mates attached to each component. Expand any part or subassembly in the assembly FeatureManager and you will find a “Mates in <assembly name>” folder directly beneath the icon for the part or subassembly. Expand the tree for that folder and you will see a short list of the mates of the parent assembly which involve that particular component.

What is the Best Way to Create a New Copy of an Existing Assembly, as Well as its Parts (Some of Which Have In-Context Features), and the Assembly Drawing?

This is often desired if you have a new design that is a modification of an old design, but you would like to manage and modify the new design separately. The easiest way is to use the Pack and Go command added in SolidWorks 2007 (see below). Here is an older method that also works:

This example will make a “-2″ version of all files while maintaining the links required by the drawing, assembly, subassemblies, parts, and in-context part features.

1. Open the drawing of the assembly “filename.slddrw”.

2. Choose File – Save As…

3. Give the drawing a new name “filename-2.slddrw” and a new folder if desired.

4. From the Save As dialog, click the References button.

5. In the References dialog, you will see the path names for all referenced files (assemblies and subassemblies). Click the Select All button.

6. Click the Replace button. Replace “.sld” with “-2.sld”. OK.

7. In the References dialog, you can Browse to a new folder if desired. OK.

8. Save.

This method creates new files with the names entered via the References dialog. The new assemblies thus created are updated to keep the in-context features pointing to the new parts, and vice versa. The new drawing thus created points to the new assembly.

Note: If drawings are not involved, this operation can be done in similar fashion from the assembly file. Choose File, Save As…, References.

A free, standalone utility called SolidWorks Explorer was introduced with SolidWorks 2000. SolidWorks Explorer makes it easier to rename and copy SolidWorks files with attention given to dependent files and where-used information.

SolidWorks 2007 added the command File – Pack and Go. This is similar to the capabilities of SolidWorks Explorer in previous releases. You have the ability to add a suffix or prefix to the file names of all associated parts, subassemblies, and their drawings. You can copy all these files to a new location with the new names using this command. Pack and Go is also available via right-click menu in Windows Explorer!

Starting a New Component in the Context of an Assembly

Most of the documentation and training material for SolidWorks focuses on creating new component parts in an assembly by using the menus: Insert – Component – New Part. You then have to select a face or plane to align the Front plane of the new component, and this creates an InPlace mate. Some users have noted a few apparent limitations imposed by this method. For example, what if the new component really needs to be affixed first via the Top or Right planes; or, what if it should be located via a vertex or an edge (for hinge or ball-joint action)?

In fact, the Insert – Component – New Part sequence is a convenience feature to save the user several steps. A more general, unconstrained method to add a new part in-context is as follows:

1. Use the New icon to create a new, empty part.

2. Save the new part with some appropriate file name.

3. Add the part to the assembly. You could do this via the menus (Insert – Component – Existing Part) or you click on the top-level icon in the part’s FeatureManager, and drag it into the assembly window.

4. Create whatever Mate relationships are desired, using the origin or any of the default planes of the empty part.

5. Right-mouse click on the icon in the assembly’s FeatureManager that represents the empty part. Choose the function Edit Part.

6. Pick a plane or face and insert a sketch to serve as the base feature of the new component.

7.  Now go to town, sketching and building features just as you would have before.

You have just duplicated the functionality of the Insert – Component – New Part function, with the important difference that you have not created any InPlace mates and have instead located the new part using one or more mates of your own choosing.

How do I save a SolidWorks generated BOM as an Excel file? 

Excel-based BOMs: Single click on the BOM so it is selected, and then go to File – Save As. Do not double-click to activate the BOM since it cannot be saved when active.

Table-based BOMs: (SolidWorks 2004 – SolidWorks 2006) Single click on the BOM so it is selected, and then go to File – Save As (or right-click on the BOM and chooseSave Template). Select save as file type Text (*.txt). Then, Browse to the saved TXT file using Windows Explorer. Right-mouse click on the TXT file and choose Open With – Microsoft Office Excel.

Table-based BOMs: (SolidWorks 2007) Single click on the BOM so it is selected, and then go to File – Save As (or right-click on the BOM and choose Save As…). Select save as file type Excel (*.xls).

How can I Locate a Component in my FeatureManager Design Tree if it is in a Subassembly?

Method 1:  Use the find utility.  Right-mouse click at the top of the assembly FeatureManager design tree and select Go to… You can type in all or part of the component’s name. Click Find Next until the component scrolls into view.  Or, from the graphics window, you can right-mouse click on any face of any component and choose Go To Feature (in Tree).

Also, you might find it helpful to change the setting in Tools – Options – System Options – FeatureManager and turn on the option to Scroll selected item into view.

Method 2: Beginning with Solidworks 2008, there is a search-filter field (shown above) at the very top of the Feature Manager in assembly files, part files, and drawing files.  Simply type your character string within this field, and as you type it will dynamically filter away all features except those that match the field.


I Want to Assemble a lot of Items onto a Common Datum Face – can I Mate Them as a Group?

Yes, this was an enhancement in Solidworks 2007.   In the Mate dialog, notice the icon that looks like a paper clip, with a lightning-bolt over the top of it – (see below), this will change the input dialog from a binary operation, (two-at-a-time), to Multi-Mate Mode.  Select the common plane or diameter for the first mate reference, then for the second selection it will allow you to group-select any number of faces of the mating parts.   Optionally, you can have all these related mates created in a common sub-folder within the Mates list for convenience.

How Can I Make Individual Part Files from a Multibody Part?

SolidWorks 2003 introduced the ability to work with multibody parts (parts with more than one continuous volume). This can be useful to develop designs that are more easily conceptualized and modeled using a single part file, but will be manufactured as an assembly of parts. This is sometimes referred to as the “master model” technique. For more information on how to do this, see the Part Modeling Tech Tips.

When I Add a New Component to One Assembly Configuration, it Appears in All of Them. Why?

This behavior is due to the default settings for assembly configurations. These settings can be changed on the fly for existing documents, and also changed and saved to your favorite Assembly Document Template for future documents. Then, components added in one configuration are automatically suppressed in other configurations.

1. Create a new assembly.

2. Activate the ConfigurationManager tab at the top of the FeatureManager.

3. Right-click on the Default configuration and choose Properties.

4. 2/3 of the way down the dialog box, notice the grouping labeled “Properties for Newly Inserted Items”. This group contains three check-boxes. The setting toSuppress Component Models should be checked. Once you check this box, components added in other configurations will be suppressed in this configuration.

5. Turn on this checkbox in your new assembly and then choose File – Save As – Assembly Document Template (*.asmdot). Save over your default template, and assembly configurations will have a more intuitive behavior.

Note: For existing files, you will need to turn on this checkbox for every configuration of every assembly if you want this behavior.

I Can’t Find the SmartMates Icon in SolidWorks 2004 or Later

One of the enhancements in SolidWorks 2004 to improve ease-of-use for assembly mating was to allow SmartMates to be applied by simply holding down the Alt key during a drag and drop operation, to snap parts together. Because of this new ability, the SmartMates icon was removed from the assembly toolbar.

However, if you prefer the older method of adding SmartMates, you can still access that older icon from within the Move Component command. Go to Tools – Component – Move, or hit the Move Component icon on the assembly toolbar. Then, at the top of the PropertyManager you will see the SmartMates icon, which looks like this:Smart Mate Icon

Click this icon to turn on SmartMates. You can now add mates to SolidWorks components by double-clicking on the first face or edge to be mated, and then single-clicking on a second face or edge to mate to. A pop-up box will then appear to confirm the mate type and alignment. Click OK (green checkmark) to apply the mate. Repeat as needed.

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