Saving Drawing Format (*.slddrt): This is concerned with company title block, logos, borders, properties and attribute links (e.g. revision, author, part number).
Saving Drawing Template (*.drwdot): This is concerned with custom drawing views, units, drafting standards, line styles, etc.

First and foremost, one must make a note of where SW is storing Template/Format files: Options > System Options tab: file location > Show folders for: Document templates or Sheet formats > take note of the location > Ok. You can Add a new location to store formats and templates, just make sure the new folder is in the network so your changes can be backed-up regularly.

Saving custom sheet format will allow you to create multiple-sheet drawings that contain company-specific format: File > Save sheet format > point to a default or custom folder in your network > Save. Now when you start a new drawing click the Browse button in the Sheet Format/Size window to point to the new format location > Ok. Notice now that when you add sheets to the drawing, the newly created format is loaded in every new sheet. You can also load the new format to already existing drawings: RMB the sheet icon in the tree > Properties > the Sheet Properties or Sheet Format/Size window appears > point to the sheet format location > Ok. This method can also be used to put different format sheets in a multi-sheet drawing.

• Create a new title block from a DXF or DWG file: File > Open > select dxf or dwg file > Open. In the DXF/DWG import window select Create new SolidWorks drawing and Convert to SolidWorks entities > Next > Show Layers: Layers selected for sheet format, select all that apply > Next > Output file properties: paper size [], Document template [drawing], Center in sheet or Position x[] y[] > Finish. Once the file is converted you can further refine the title block by: RMB > Edit sheet format.
• You can createa title block that passes property data to the part file: RMB > Edit sheet format > RMB > Define Title Block > create a bounding box around the sketch defining the title block > select the text fields that you'd like to use > Ok > Exit Edit sheet format (RMB > Edit sheet). Now when you create drawing views of a part just 2x-click the title block and enter the data that will be passed to the part properties.
• To insert a logo or picture in the title block: RMB > Edit sheet format > insert > Picture > select a file (bmp, gif, jpg) > Open > Modify picture to adequate size and position > Ok > Exit Edit sheet format.
• Define and ancor point for a table (e.g. BOM, revision, weldment): RMB > Edit sheet format > select a point > RMB > Set as Anchor > select a table > RMB > Edit sheet.
• Linking title block text with part properties: within the drawing sheet RMB > Edit sheet format > add a note in the target cell or click the available note already there. Next, in the Note properties window: Text format > Link to Property > in the Link to Property window select Modified view specified in sheet properties > From the drop-down menu select the desired property > Ok > Exit sheet format. You can also link to properties of the drawing itself (e.g. current sheet, total sheets, scale, date): in the Link to Property window select Current document > select the property.

Saving custom sheet template: File > Save as > point to a default or custom folder in your network > enter a name and choose Drawing Template (*.drwdot) file type > Save. Note that to save a template one doesn't need to have a sheet format specified, so the template could be a blank sheet to which a predefined sheet format is loaded later.

• Changes to template units, dimension standards, line styles, etc. can be changed at: Properties > Document Properties tab > Make changes > Ok.

• Autodimension will quickly place dimensions for all features: Tools > Dimension > Smart > Autodimension tab > select a Horizontal and Vertical reference lines in the drawing view > apply > Ok.
• Importing part dimensions created with DimXpert: click the drawing view > in the PropertyManager menu > Import Options: DimXpert annotations > Ok.
• Model Items function can insert dimensions, annotations, and reference geometry from a model document (part or assembly) into a drawing: insert > Model Items > select relevant options >Ok.
• Format painter allow you to copy the settings of a dimension to another dimension by simple click: Tools > Format Painter > select the dimension whose properties you want to copy > select the dimension you wan to change > RMB exit.

Rotate a 2D view along an axis perpendicular to the paper: Rotate drawing view > drag or enter the rotation angle for the view > apply > close.

The Wrap feature allow to easily create geometry in the surface of cylindrical objects: for this example create a (1) cylinder, extrude it and (2) create a reference plane that is parallel to the (3) one cutting through the middle of the cylinder and (4) tangent to its circumference. (5) We then create a global variable containing the diameter value of the cylinder so we can refer to it later. R-click the dimension > link values > enter name of the Global variable (e.g. Dia) > Ok. In the new plane, create the geometry that will wrap around the cylinder, matching the circumference. Make the length of the sketch equal to Dia*pi. To implement the Wrap function: insert > features > wrap > select the sketch > select the cylindrical face > select emboss, deboss or scribe, this last one will just split the face > enter the depth > Ok. This is a good opportunity to try using Equation Driven Curves to create accurate geometrical sketches: Tools > Sketch Entities > Equation Driven Curves.

The Wrap function is also ideal to create embossed/debossed lettering in solid objects. However, the letters and its frame should be contained in two different sketches. A sketch containing other closed loop sketches can be embossed/debossed in one single Wrap application.

The Decal function provide a way to put the equivalent of sticky labels on the surface of planar and curved objects: You can grab image files such as jpg, bmp, png, etc. from the Decals folder and drop them on the object. You can also upload custom decals using the Edit Decal function. The function is located in the Rendering tools ribbon. The ribbon can be activated by: View > Toolbars > Render tools.

Rotate a body or set of bodies to match the default isometric view: select all bodies in the assembly > Tools > Component > Rotate > select to rotate either by Free Drag, About Entity, or By Delta XYZ.

• Free Drag: LMB and rotate the object to position > Ok.
• About Entity: Select a line of other entity > rotate to position > Ok.
• By Delta XYZ: enter an angle increment in one or more of the X,Y, or Z axis > Apply >Ok.

The Indent function uses a body as a tool to create an indentation in another body. First, create and position a separate body to use as a tool: insert > feature > indent > select the Target body, select the Tool body region minding which side of the body you click on, as represented by the black dot (see figure above). This determine which way the indentation is applied. Specify a Thickness and Clearance as needed. Use the Cut options to create a hole instead of an indent > Ok. You may also check Remove selections or hide the tool bodies to complete the effect.

The use of cosmetic threads can save time and memory usage in your computer. Cosmetic threads (C.T.) can be applied to holes and shafts. Go to Insert > Annotations > Cosmetic Thread... > select the edge of the feature you intent to tap and fill out the settings in the C.T. window. Tapped holes should be made at minor diameter and shafts should be made at major diameter size. SW C.T. window will only display thread size options for those corresponding to the selected geometry diameter. Make sure the file is set to display cosmetics threads by going to Options > Document Properties tab > Detailing > Display filter: check Shaded Cosmetic threads box > Ok.

Keeping track of patterns containing large amounts of holes in SW 2013: Combine Hole Wizard and the Fill pattern functions to create and keep track of patterns with large number of holes. First, create a hole through the hole wizard, then > Insert > Pattern/Mirror > Fill pattern > enter the necessary parameters > Ok. Once the drawing file is created just use the Hole Callout function to retrieve the hole count just created (Insert > Annotation > Hole Callout). Later SW versions may contain functions to check the hole count in the part/assembly modules, and not only the drawing module.

Decals are preferably applied at the single component level, not assemblies. Click the Display Manager tab located next to the history tree. Next, click the Decal icon and Right-click on the grey area below the Open Default Library button > Add decal. Click the Browse button and locate the file you want to use (jpeg, PNG, etc.) the click the surface you wish to place the decal on. Click the mapping tab to access controls to rotate, change size, and make other changes in the image.

You can clear out the background color of your decal via Selective Color Mask or Image Mask File. The image mask require saving a copy of the original decal as a Monochrome Bitmap file. then browse to the location of the Bitmap > click the Inverse Map check-box > Ok.

• AssemblyXpert analyses assembly performance and makes recommendations for improvement. Tools > AssemblyXpert.
• Have the least amount of top-level-assembly mates as possible.
• Increase the amount of sub-assemblies at the top level.
• Top-level assemblies do not solve sub-assembly mates, unles you make sub-assemblies flexible. R-click a sub-assembly in the Feature Manager tree > select Component Properties > solve as > flexible > OK.
• Light Weight Components is no longer the prefered method to view large assemblies. Tools > Large Assembly Mode. Open file > choose file > mode >lightweight.

• This is the fastest way to view a very large assembly
• Open only the components you need (selective opening)
• You can Hide/Show parts, create sections, Measure, Add Walk thru
• Open file > mode > Large Design Review > This loads a lighter component tree and a Review Toolbar.

• Prevent external reference creation: tools > options > External References > Do not create references external to the model.
• Suspend automatic rebuild: R-click assembly tree > Suspend Automatic rebuild
• Store files locally
• Tools > Options > Performance > check-off transparency settings, lower curvature generation, change fast animation speed.
• Tools > system options > assemblies > change settings accordingly.

• Quickly create a simplified version of large complex assemblies without losing graphics detail.
• Reduces memory usage
• Maintain references
• Works in drawing mode by transfering complete BOM list and annotations capability
• You can speedpack another Speedpack file.
• You can share Large-assembly files without giving away all parts information.
• From an assembly file > configurations > R-click on the desired configuration > add speedpack include only faces useful for mating and dimensioning. The remainder will be visible as ghost > Ok.
• From the top-level assembly > select sub-assembly > R-click > Speedpack Options > Create mated speedpack: this will only load the faces necessary to create a light version of the assembly that is fully visible.

• Use instead of Configurations when all is needed is to exclude a component to display or change transparency or color.
• Never require a re-build
• They are listed at the bottom of the ConfigurationManager
• To create a new display state: Click a blank area in the graphics area to make sure nothing is selected in the ConfigurationManager. R-click in any blank area in the ConfigurationManager and select Add Display State. A new display state is added to the list and becomes the active display state. In the FeatureManager, click ">" (to the right of the tabs) to show the Display Pane, and make changes to define the new display state.

Feature Statistics is a tool that display the amount of time it takes to rebuild each feature in a part. Use this tool to reduce rebuild time by suppresing features that take a long time to rebuild. This tool is availble in all parts documents. Tools > Feature Statistics. Tip: Add a configuration specifically for Simplified versions of a part.

• Insert > Features > intersect... creates volume (solids) by creating an enclosure of surfaces and reference planes.
• Insert > Cut > Extrude... can be used to sculpt away pieces of a solid using a line.
• Insert > Cut > with surface.. removes material from either side of the surface.
• Insert > Surface > Boundary Surface... create a surface from two intersecting splines.
• Insert > Curve > Projected... Combine perpendicular sketches into one 3D curve or project a sketch unto a surface.
• To save a Solid as a separate part file: Select the solid > R-click > insert into new part... > give it a name.

Downloading weldment profiles: Design Library tab > Solidworks Content > Weldments > Ctrl & L-click the package you want to download > specify a folder location > Ok. The download may take a few minutes. Once the zip folders are done, extract the files and then locate the default folder where solidworks keep weldment profiles in order to place the extracted folders there. This is how you can find the location: Tools > Options > System Options [Tab] > file locations > Show folder for: weldment profiles > make note of the location (copy it) > Ok. When placing the new files in the default folder be careful with name conflicts [e.g. ANSI inch folder repeated twice]. Once this is done the new profiles should be available in the Structural Member selection window.

Creating custom weldment profiles from imported DXF/DWG files: Start a new part file > select a plane > Insert > DXF/DWG > select the file > in the DXF/DWG Import - Document Settings window: 2D sketch, import dimensions, merge points closer than [0.1] > Finish. To adjust the position of the imported sketch: Sketch [tab] > move entities > select the geometry, check From/to, select the origin and destination points > close sketch editing. Now save the imported sketch into the appropriate Weldment Library location: select the sketch > file > save as > choose file type: Lib Feat Part (*.sldlfp) > browse to the file location as explained in the previous paragraph and create a new folder if necessary > assign a good descriptive name [e.g. 45x45x0.25] > OK. Another way to save the profile is: R-click the profile > Add to library.

Placing Structural Members: Note that splines cannot be used to place weldment profiles. Once yo have chosen a weldment profile and select the 3D lines that define the structure, you can change the point in the profile in which the normal alignment occur: in the Structural Member window > Locate profile > select a new point in the profile. Profile-point-of-alignment location can be used as a good rule to go by when creating weldment groups: if a structural member is expected to share the same profile point then they should be place in the same group. You can change the corner treatment by R-click an individual point and select from the options available. Also, the weldments can be rotated, aligned and mirrored about the profile point by entering the information in the Structural Member window.

To create an exploded view of a weldment: in the configurations tab > R-click in the weldment icon > New exploded view > move members to the desired position > Ok. You can also go to insert > Exploded view.

Update the cut list so all similar parts can be grouped together: Once all the weldment parts are in place R-click the cut-list icon in the tree > Update. To hide/exclude an item from the cut list, expand the cut-list icon in the tree, R-click specific weldment part icon > exclude from cut list.

Entering property information for end-caps, gussets, panels, etc.: R-click the weldment group that needs editing > Properties > in the Cut-List Properties window enter the information needed > Ok. One way to take advantage of the parametric nature of the parts, such as a square plate is to use the dimension variables to write the description of the part that appear in the cut list. In this manner if the part was to change in future revisions, the description will also change automatically: make the 3D dimension visible by 2x-click the feature > click the dimension to enter its name in the properties row (e.g. ″D1@sketch1″ x ″D1@sketch2″ x ″D1@sketch3″ translates to 45 x 45 x 0.25) > Ok. If you just want to include the stock size material needed to create a gusset, for example, the bounding box information can be inserted as follows: R-click the folder containing the gussets > Create Bounding Box > R-click Cut List icon > Update. This will populate the DESCRIPTION section of the cut list.

Insert a cut-list into the drawing: Annotations > Tables > Weldment Cut List > select the view on which the list will be based > enter other properties > Ok. To insert a new column to either side of the selected one, place the cursor over the column > R-click the blue cell > insert > Column Right/Left. To assign a property to this particular column: L-click the top blue cell in the column > in the Column Properties check Cut list item property > select the item > Ok.

Linking Drawing view to BOM or Cut List: in the 2D drawing R-click the source view > Properties > View properties [tab]: Balloons, link balloon to the specific table > choose the list you want > Ok.

Inserting a 2D view of ONLY ONE weldment member: Insert > Drawing view > relative to model > this will take you back to the part file > In the Relative View window: Selected bodies > select the member you want in the view > select the first and second orientation references > place the new view in the 2D drawing.

To create a Base Flange: sketch an open or closed profile sketch > insert > sheet metal > base flange > select the profile sketch > enter appropriate parameters such as Bend Allowance and Auto Relief > Ok.

To convert a solid to a sheet metal feature: insert > Sheet Metal > Convert To Sheet Metal (CTSM) > in the CTSM window select a fixed entity, this is the part that remain stationary during unfolding of the part > select Bend Edges around the fixed entity > continue selecting bend edges and managing the Rip Edges accordingly > Ok. You can also include sketches to be used as custom rip edges, just select the sketch and place it in the Rip Sketches option of the CTSM window.

Lofted-Bend function is primarily used to create duct work of changing profile. The following are prerequisites to creating Lofted-Bend features: (1) only two sketches per part,(2) sketch profiles must be open (aligning the openings in both profiles is good practice),(3) no sharp corners on the profiles. Once the profiles are in place: insert > Sheet Metal > Lofted-Bend > select the profiles > specify the Faceting Options which control the transition bends between the profiles > specify other parameters such as thickness, K-factor, manufacturing options, etc. > Ok.

The Edge Flange function creates an extended edge/tab from the edge of a another flange one straight flange at a time: insert > Sheet Metal > Edge Flange > select an edge and enter angle, length, and flange position > Ok.

The Miter Flange function is similar to the Edge Flange, it adds a series of flanges to one or more edges of a sheet metal part with the added option to include a custom profile. The function will avoid curved edges and only extrude an flange profile drawn perpendicular to the flange edge: insert > Sheet Metal > Miter flange > select a face (perpendicular to the edge) to start a profile sketch > draw a sharp-corner open profile of the flange > Ok. In the Miter Flange window select the edges you need and enter other parameters such as Start/End Offset > Ok.

The Hem function can be used to create hinge features and folded ends: insert > Sheet Metal > Hem > enter type and size > Ok.

The Jog function will create an offset section usually located near the edge of a flange: create a sketch line along the edge of the flange > insert > Sheet Metal > Jog > select the sketch > select the fixed face > enter the jog offset, Position, and Angle parameters > Ok. Meanwhile the Sketched Bend function allow one to sketch a custom bend line in the part: insert > Sheet Metal > Sketched Bend > create a sketch > Ok > select the side of the sketch that will remain fixed > enter the bend position, angle, and radius > Ok.

The Cross-Break function creates a representation sketch and notes of a reinforcing bend commonly used in duct work. The 3D model is not affected but the fabrication notes are included in the 2D drawings: insert > Sheet Metal > Cross Break > select the face > one can edit the sketch profile if needed as well as the angle and radius > Ok.

The Closed Corner function will effectively close any gaps created by the bend allowance on flanges that are perpendicular/parallel to each other: insert > Sheet Metal > closed corner > select perpendicular faces, select Corner type, and make sure Coplanar faces and Narrow corner options are checked > Ok.

The Welded Corner function will put a weld fill between two perpendicular flange faces. The flanges must have the same length: insert > Sheet Metal > Welded Corner > select face 1 and 2 > Ok.

The Break corner-Corner trim will create a fillet or chamfer in a single flange part: insert > Sheet Metal > Break corner-Corner trim > select edge > select Break type and distance/radius > Ok.

The Corner Relief function allow you to specify a particular relief shape to each corner in the same part: insert > Sheet Metal > Corner Relief > the Collect all corners button will display all accessible corners as orange-color dots > assign each corner its relief option: rectangular, circular, tear, obround, or constant width > Ok.

The Sheet Metal Gusset function places a formed gusset in a bended corner to increase the stiffness of the part: insert > Sheet Metal > Sheet Metal gusset > select the two faces and enter other parameters such as dimensions, fillet options, draft angle, etc. > Ok.

The Forming Tool function create sheet metal features that simulate a punching/stamping operation. First, one must create the tool: create a part in the shape you need > insert > Sheet Metal > Forming Tool > select the stopping face and faces to remove (the removing part is optional) > Save the part in the library, preferably the forming tools folder. The folder is formatted to recognize parts as forming tools. R-click the forming tools folder > check there is a check mark specifying so. Second, to use the new tool just drag it from the library into the surface of the sheet metal part > specify: placement face, rotation angle, configuration, position > Ok. You can link the resultant feature to the forming tool so changes in the tool will be reflected in the form. The steps of using the forming tool are illustrated below.

To create a vent feature in the sheet metal: create a sketch of the vent > insert > fastening feature > vent > select the Boundary line, the Ribs lines (across the diameter of the boundary) , the Spars (concentric to the boundary), and the Fill-in Boundary (center) > Ok.

A fill pattern function can also be used to create venting features in a part. Before creating a fill pattern feature one must define the area where the pattern will be located. This is done by splitting a surface using a sketch: insert > curve > split line > select the sketch defining the boundary and then the surface you wish to split. To create the fill pattern feature: insert > pattern/mirror > fill pattern > select the fill boundary area > enter the parameters defining the pattern > Ok.

To create an exploded view of a multi-body sheet metal: in the configurations tab > R-click in the weldment icon > New exploded view > move members to the desired position > Ok. You can also go to insert > Exploded view.