Rounded Corners

When dimensioning corners that are rounded the is no need to dimension the center location of the arc. Instead dimension the edges and the arc radius.

Outline Consisting of Arcs

Sometimes your outline will be pretty complex, made up of nothing but arcs. To dimension an outline made up of arcs first ensure that each arc radius is called out. Then the necessary center locations should then be dimensioned. Care should be taken when dimensioning outlines so that it is not over-dimensioned. There will be times that the location of some arcs will not need to be dimensioned since it’s location is fully defined by it’s tangencies.

Irregular Outlines

Irregular outlines can be extremely troublesome to dimension. An irregular line can be made up of a spline that can’t be dimensioned by conventional methods. Instead, the best way to do it is to place points on the line that can then be dimensioned coordinately. I find ordinate dimensions work best for this situation sense it is often cleaner, but that is a personal preference. ASME Y14.5 also allows designating each point with a symbol, such as a letter, that is then referenced in a table. This was great in AutoCAD or manual drafting but I do not encourage it in SolidWorks, since as the outline changes the values will not be updated in the table.

Symmetrical Outlines

In my opinion, this is one the aspects of ASME Y14.5 that really doesn’t apply in today’s CAD world. In the past when drawings were hand drawn, a great time saving practice was to only show one-half of a large profile that was symmetrical. The centerline for symmetry designated that the unseen portion of the profile was a reflection of the shown outline. The profile centerline was then designated for symmetry with two thick horizontal lines, looking like a an equal sign, at the top and bottom of the centerline. Refer to ASME Y14.2M for more information on this linetype.

Round Holes

The illustration below shows how to dimension a round hole. When the depth of the hole is not obvious then it must be dimensioned. If the hole goes through the entire feature then the abbreviation of THRU may be used to follow the diameter. When the depth is a blind depth, most of the time you can get away with using the depth symbol shown below. If the depth is not clear, as when you are dimensioning a hole on a cylindrical face,  specify the depth with a dimension.

Slotted Holes

Slotted holes can be dimensioned as shown below. If using the DimXpert, each of these methods are supported. However when dimension by using conventional methods you may find the Ex. 1 & 3 are easier.

That will cover it for today. I realize it is extremely short but to be honest I ran out of time. Next week, I will make sure that my continued converage of ASME Y14.5 is a lot better. Hey, it’s like they say it’s not the quantity, it’s the quality.

What is The Feature Selector?

For today we will be taking a brief look at the Feature Selector. The Feature Selector is another of those newfangled context toolbars that everyone has been talking about. The Feature Selector is used to differentiate between the various DimXpert feature types depending on the face that is selected and command being used.

The Feature Selector toolbar is available when you select a face for dimensions, datums, geometric tolerances, automatic tolerancing schemes, and pattern creation. From left to right the features shown in the toolbar reflect the complexity of the selected feature. The feature on the left side of the toolbar are the most basic, including planes, cylinders cones. In the middle of the toolbar slightly more complex features including patterns, notches and counterbores are shown. Finally, on the right are the most complex feature types including intersect points and lines and compound features that require more selections.

Supported Features

Below is a list of the various supported features that may be shown on the Feature Selector. Some require some explanaition but a few of them are pretty straight forward.

Boss

A boss is a extruded cylinder whose face is completely 360°

Cone

A cone is any conical face that is either internal (hole) or external (boss).

Chamfer

A chamfer can either be a conical surface, as shown below, or a planar surface.

Cylinder

A external in internal cylindrical face that is a full 360° or a partial can be a cylinder. However if the cylinder is a full 360° it my only be able to be considered a boss, as described above.

Fillet

Counterbore Hole

A counterbored hole will be recognized by DimXpert as long as it does not have a near side countersink or head clearance. If your counterbore meets one of these two conditions you will need to dimension each element individually as a cylinder or hole.

Countersink Hole

A countersunk hole will be recognized by DimXpert as long as it does not have a far side countersink or head clearance.

Simple hole

A simple hole can be threaded or non-threaded, through or blind, with a flat bottom or drill tip or even a compound hole.

Intersect Line

An interest line is a line created by the theoretical intersect of two planes use for dimensioning.

Intersect Plane

An intereserct plane is created when selecting a cyliner and a conical face in order to locate the begining or ending of a tapered surface.

Intersect Point

Intersect points are shown as origins when selecting a cylinder or hole and a plane. This can then be used to locate the position of the hole using a dimension.

Notch

Plane

Slot

Width

Well that about covers it for the Feature Selector. I know that there is a lot of material to cover, that is exactly why I am breaking up everything into parts that will then be tied together at the very end. So be patient and everything will make sense later. As I mentioned earlier, to avoid complete overload we will be jumping around to other topics over the next couple of days and we will probably pick up once again on DimXpert early next week.

Datum

Before applying dimensions to your part is a good idea to identify your primary datums. In the DimXpert tab of the CommandManager click the Datum button.

In the Datum Feature FeatureManager enter the datum label and select the leader type.

Next select either a boss, cylinder, notch, plane, simple hole, slot or width you wish to designate as a datum.

With your datums assign you may next move on to the assigning tolerances and dimensions.

Size Dimension

After identifying the primary datums in the part it is time to start adding dimensions. In the DimXpert tab, select the Size Dimensions button.

The Size Dimension tool will support applying dimensions to bosses, chamfers, cylinders, fillets, counterbore holes, countersink holes, simple holes, notches, slots and widths. With the Size Dimension tool active select the feature to be dimensioned.

Pattern Features

DimXpert will recognize most patterns and automatically specify the number of instances of a select feature. For example this models has four screw holes then when dimensioned the DimXpert adds ’4X’ preceding the dimension.

Tolerances

The default tolerance value for diameters, slot and notch lengths, counterbore diameters, countersink diameters, widths, depths, countersink angles and fillet radii can be set in the Document Properties in DimXpert -> Size Dimensions.

After placing a dimension the tolerance can be modified in the DimXpert PropertyManager just like when placing dimensions in a drawing.

Grouping

When you place a dimension on a feature that was previously defined with a datum, geometric tolerance, or other annotation feature then the DimXpert automatically groups then into an annotation group.

Depth Dimensions

Depth dimension will only be applied to features that are blind. There are other criteria that effect whether or a not a depth dimension is applied such as the end condition of the blind feature.

Threaded Holes

Threaded holes that are created with either the hole wizard or cosmetic thread will be dimensioned with the thread designation.

Location Dimensions

The Location Dimension tool is used to dimension between two existing DimXpert Features with linear or angular dimensions. This tool cannot be used to apply dimensions to surfaces, fillets, chamfers, and pocket features. First click the Location Dimension button in the DimXpert tab.

Next, click between two features and place the dimension. In this example, we are placing the dimension between the center hole and one of the outer holes.

Over the next couple of post I will continue to dig more into DimXpert. As you can tell, despite being a fairly easy tool there are alot of areas that should be addressed. Be sure you subscribe to my RSS feed so you can be certain that you will not miss any exciting update. Until later, have fun with SolidWorks and be certain to ask me any questions you may have.

Diameters

When dimensioning a diameter you must precede the number value with the diameter symbol, shown below. I have seen some people try to sneak in the acronym DIA., but that doesn’t fly around here mister. Besides, if you are using SolidWorks you just have to click the diameter symbol in the PropertyManager. If you need to specify a spherical diameter, once again don’t type in SPHERICAL or any other variation, use the spherical diameter symbol shown below. In SolidWorks you can just plop an ‘S’ in front of the diameter symbol but this not exactly correct since it would create a space between the two. Instead use the Symbol Library to insert the Spherical Diameter symbol.

When dimensioning multiple concentric diameters, it is better to apply dimensions from the side view. Of course, this is not a rule, it is just good practice. Dimensioning a part from the front, looking directly at the diameters, could get confusing as to what dimension applys to which diameter.

Radii

As with diameters, when you dimension a radius; the radius value must be preceded with the appropriate radius symbol. Each radius dimension uses one leader and one arrow pointing to the arc. When a the position of the center of the arc is critical a dimension line is to be drawn from the center to arc with the dimension between the two, as long as space permits. When space is an issue extend the line beyond the radius center. When you do not dimension the center of the arc then center marks are ommited and the arc is controlled by other means such as the tangent surfaces. If you do dimension the center of the arc use a small cross to represent the center.

Foreshorten radii

A foreshorten radius is used when the center of the dimensioned arc extends beyond the limits of the drawing or the dimension may interfere with another dimension. In SolidWorks this is done by clicking the Foreshortened button in the Leaders tab of the Dimension PropertyManager.

The radius dimension is then foreshortened. When you dimension the centermark of the radius the dimensions will be foreshortened as well.

True Radius

When you are dimensioning a radius in a view that is not reflect the true shape of the arc the word TRUE precedes the arc dimension. In SolidWorks this is done automatically when you place the dimension but it may require some massaging.

Multiple Radii

When you are dimensioning multiple radii of the same radius you may dimension one of the radii and precede it with the number of times, as in 3X R.125.

Spherical Radii

As with spherical diameters, when you are dimensioning a spherical radius the dimension is preceded with SR. This however does not need a special symbol from the Symbol Library.

Chords, Arcs and Angles

Chords, arcs and angles are dimensioned as shown below. Chords and angles are simple to dimension but dimensioning an arc tends to be a sticky point for a lot of people. In SolidWorks, to dimension an arc with the dimension tool active click the arc. Then while holding down the CRTL key, click both of the end points of the arc.

Rounded Ends

The image below illustrates the techniques for dimension features that have rounded edges. First dimension the overall dimension by holding down the SHIFT key in SolidWorks and clicking both of the arcs. When the arcs is a full radii,only indicate the radius but it is not dimensioned. When the feature has partial radii, then they are dimensioned.

Well, I think that will do it for today. Next week we will continue all the fun. Until then, I hope you are making even better drawings with the information I have shown you today and all of the previous Standard Tuesdays. As always, I will always be here to help you with any questions you may have.

Auto Dimensioning a Simple Part

In our simple part, select the DimXpertManager tab in the FeatureManager.

In the DimXpertManager click the Auto Dimension Scheme button.

In the Settings section select whether your part is a Prismatic or Turned part. A Prismatic part would be most likely machined using a mill and a Turned part is most often done with a lathe. Since our part is a simple block with a full holes and a groove, we will select Prismatic. Next, select what type of tolerance will be applied. If you are like most people you might want to pick Plus and Minus but give me a few weeks and you’ll jump into the Geometric tolerancing like a pro.

Next, we will select our Datum References. Every part is different and you have to think about how the part will be inspected by your quality control department. In this case, we want our datums to be the back, top and left planes of the part. These are considered mutually perpendicular planes and provide a good origin.

You will notice that the planes selected are color coded to match the Primary, Secondary and Tertiary Datums.

Select the Scope of the features you wish to be dimensioned. Since this is a simple part we can get away with selecting All Features, more complex parts may require you to individually select which features to be dimensioned. In the Feature Filters section, Select the features types that you wish to be recognized. Deselecting a feature type will cause all those features to be omitted from the calculation.

When you are finished with your selections, click the green check mark and the part will be fully dimensioned. The created dimensions are based on the actual geometry of the part and are not based on sketch dimensions. Depending on the complexity of your part you may find it necessary to change your layout for readability but since this is a simple part it is not necessary here.

Creating a Drawing from a Dimensioned Part

Even though, per ASME Y14.41, you do not need to create a drawing your company standards may still require you to do so. The best thing about using the DimXpert for parts, the work is already done for you. When you insert the model into your drawing select DimXpert annotations in the Import Options section and the drawing will be created with the annotations you created.

Now all you have to do is arrange your dimensions for optimum readability and you done. Too easy!

Now like a mentioned is is just a quick introduction to the DimXpert for parts. In future post I will be digging deeper into this powerful tool and show some cool things you will be able to do. SO make sure you stick around.

I realize that since I have been asking my readers to subscribe to my RSS feed, that some of my less tech-savvy readers might not know what that means. A RSS feed, Really Simple Syndication, delivers blog entries, News Headlines and Podcast to an aggregator or RSS reader; in most case for free. For example, subscribers of The SolidWorks Geek RSS Feed receive in their reader the latest published post usually within a few minutes after it is published. This will keep you up to date on all your favorite blogs that you you have added to your own aggregator without having to visit the site itself.

Finding Your Own RSS Reader

There are a number of free web-based or desktop-based RSS readers, each with it’s own pros and cons. I currently use Google Reader but I am slowly moving my feeds to Netvibes on the advice of Ricky Jordan. Just because you pick one reader doesn’t mean you are stuck with it. There is nothing keeping you from having a few different readers to help figure out which one works best for you but I hope you add The SolidWorks Geek Feed to each of them .

Below is a list of the some popular aggregators, readers, available for free:

• 
• 
• NewzCrawler
• FeedDemon
• NetNewsWire

Wikipedia has an awesome list of RSS aggregators here.

Subscribing to a Feed

Many blogs, including The SolidWorks Geek, uses an icon somewhere on the page the represents the RSS feed. Every icon will look different but they all have a common element, the symbol for RSS.

Clicking this icon will take you directly to the feed content page. This page will look different depending on how the blog set up its feed. I use Feedburner for my feed but that is a different post.

From this content page you will be able to select the reader you use and it should add the feed automatically. If your reader is not listed or the page doesn’t list any readers, you can copy the page URL from the address bar use CTRL-C.

Then paste the URL into your reader.

Well, folks that was a quick introduction to RSS feads. Hopefully now you will feel compelled to subscribe to my feed and you might just win a cool prize. I hope everybody has a great 4th of July weekend and I will see everybody on Monday!

Add Balloons to Drawing

Today I won’t spend too much time on adding balloons, or item identifiers, to the drawing. We will save that for a different day and a different post. Since this is a real simple assembly we can just go with the AutoBalloon tool in the Annotations toolbar.

Clicking our isometric view we now have balloons attached for all the components… or do we?

Where is the BOM Content Command?

Previous to SolidWorks 2008, you were able to click the BOM Content button in the PropertyManager for the select BOM. The BOM Content window allowed you to view the components in your BOM, see what components are missing balloons, see the type of components listed or reorder the items in your BOM. All that functionality is still available but instead of being a separate window it is now part of the BOM itself.

Viewing the Balloon Status and Assembly Structure

One of the functionality of the original BOM Content window was viewing the Balloon Status and Assembly Structure. Now you can view these directly in the BOM, nice and easy. Click the expansion arrows on the side of the BOM, the tree tiny little arrows pointing out from the BOM, and addition columns will be show.

In this view, we can quickly see which components have balloons attached to them. If we missed any, we should go back and make sure they are added. In this view we can also see the assembly structure. Since we currently have our BOM to show only parts we only see part icons with no real structure.

If our assembly was set to Indented Assemblies we would be able to see the full structure along with the component type icons.

Reordering the BOM

Another functionality that was originally available in the BOM Content window was the ability to reorder the BOM. I am personally glad that SolidWorks got rid of the window since now you can reorder the BOM in the BOM. How cool is that? It couldn’t be any easier, select the entire row at the row number…

…and drag the row to the desired location. Too cool!

Of course you cannot change the order of the BOM when you have Follow Assembly Order selected in the right-click menu. When you select Follow Assembly Order the only way to change the order of the components in the BOM is to reorder the assembly structure.

Splitting the BOM

As your BOM grows, it may become too large to fit vertically in your drawing. In this case, you want to split the BOM and move the second part somewhere else in the sheet or even another sheet. In the BOM select the row where you wish to apply the split and right-click. Select Split from the menu and select one of the options; Horizontally Above, Horizontally Below, Vertically Left or Vertically Right.

You can now drag the second section of the BOM anywhere you want. You can even use Cut and Paste to place it onto another sheet and it will remain linked.

To combine the two BOMs back into one, select Merge Tables from the right-click menu.

Insert a New Part

You can now add new parts directly from the BOM using Virtual Components. First, right-click the BOM and select Insert New Part.

This will insert in a blank line into your BOM. IF you expand the BOM you will see that new item is a Virtual Component shown with brackets, [ ].

In your assembly you will see the new virtual component added to the FeatureManager. We will be covering Virtual Components at a later date.

I hope you will find, after reading this, BOMs extremely helpful and easy to use. I encourage you to explore BOMs more in the future since there are more tools built into the BOM. If you enjoyed this post and all the other Tips and Tricks I offer here at The SolidWorks Geek, please subscribe to my RSS feed and you might just win our contest.

Chain Lines

As mentioned in Rule 11 of the Fundamental Rules of Dimensioning:

“Unless you specify otherwise on the dimension, it should apply to full depth, length or width of the feature.”

When it is not appropriate to have the dimension apply to the full depth, length or width of the feature; chain lines allow you to indicate a limited length or area of a surface. You can use chain lines to apply treatment to only a section of a feature. A good example of this is when you want to add knurling to only a section of a shaft.

Applying Chain Lines

In the view that best describes the location and extent of the surface to be prepared draw a chain line parallel to the object line offset a small distance from the line(s). Add dimensions to show the length and location of the chain line if it is not clearly indicated by the mere location of the line. If you are adding a chain line to a revolved part, you can show the line on only one side of the feature. If you are apply chain lines to a view that is normal to the reader then you create a fully dimensioned boundary using chain lines. Below illustrates applying a chain line to a shaft:

Leaders

Leaders are used for local notes, symbols and some types of dimension such as diameters and radii. When pointing to an edge or point of an object, the leader should terminate with an arrow head. When pointing to a surface the leader should terminate with a dot, which indicates that the entire surface within the object line boundary is being indicated. Leaders can be drawn using straight lines at any angle but to maintain readability of the drawing, adjacent leaders should be drawn parallel to each other. The other end of the leader, the short horizontal line, should point to the middle of the first or last character of the note or dimension.

Leader Directed Dimensions

Leader Directed Dimensions such as radius callouts should be drawn individually. Although SolidWorks may give the ability to have multiple leaders when make dimension callouts it should be avoided since it adds an unnecessary degree of complication to the dimension. Also, if your drawing view contains a lot of radial dimension that may make it difficult to read, you should use flagnotes or letters to identify the dimensions elsewhere on the drawing.

Circle and Arc

When dimensioning circles and arcs, the leader must be drawn radially. In SolidWorks, this is not an issues since it automatically creates all radius or diameter dimensions radially. Making a leader radial means that if you were to theoretically extend the leader line it would intersect with the center mark of the arc or circle.

Reading Direction

The reading direction of all notes and dimensions must be consistent throughout the drawing. After all we are not doing architectural drawings here. All notes and dimensions must  be able to be read without having to turn the drawing around other then the intended direction based on the format. The one exception to this is when you are using ordinate dimensions, which are meant to be inline with the extension line. Ordinate dimensions will either be read from the bottom or the right based on whether they are vertical or horizontal. Ordinate dimensions will be discussed in detail in a future Standards Tuesday post.

Reference Dimensions

Judging by the drawings I see at my day job, everybody knows how to specify a reference dimension. Even though most don’t know how to use them properly :0). Anyway, specify a reference dimension by enclosing it within parenthesis. As I mentioned in an earlier an earlier post, reference dimensions should be used sparinly.

Overall Dimensions

An overall dimension is used to show the entire length, width or height of a part including all of the intermediate dimensions. If you do use an overall dimension then one of the intermediate dimensions must be left out of the view or shown as reference. This is because if you left all the intermediate dimensions along with the overall dimension the part would be over constrained. If it is more important to show the intermediate dimensions then the overall dimensions must be as a reference.

Dimensioning Within the Outline of a View

If at all possible, always make every attempt to place dimensions outside of the visible object lines of the drawing view. Of course there are times when this is near impossible, either because of the feature being dimensioned or the length of the extension lines. When this is the case, dimensions can be placed within the visible object lines.

Dimensions Not to Scale

Even though the writers of ASME Y14.6M-1994 make every attempt to be diplomatic, I will not. This is a huge thorn in my side when I deal with drawings from other users. With out sugar-coating it, there is no real reason to have a drawing not be done to scale when using modern CAD packages. The only excuse would be….laziness. I have a feeling I will receive a bunch of emails about this.

Well, that concludes Section 1.7 Application of Dimensions as described in ASME Y14.5M-1994. Like I said, next week we will begin coverage of the methods of dimension features. Until then, feel free to contact me with any questions, comments, or complaints. If you enjoy reading the SolidWorks Geek and you don’t want to miss anything please subscribe to my RSS feed. Its free, easy and it just might earn you a prize.

Inserting BOM into Drawing

To insert a BOM into a drawing click Tables -> Bill of Materials in the Annotations toolbar. I use the Shortcut Bar almost exclusively, to bring up the shortcut bar select ‘S‘ on your keyboard. For more about Shortcut Bars refer to: Improve Productivity – Use Shortcut Bars.

After clicking the Bill of Materials button you will be prompted to “Select a drawing view to specify the model for creating a Bill of Materials.“. You may select any view but I would recommend select the primary view in your drawing, usually the isometric will work. What ever configuration and display state is shown in the view will be used to populate the BOM.

After selecting the view used to populate the BOM you will be prompted to select the options for the BOM. We covered all of the options last week, feel free to go back before continuing on.

Once all your options have been set, click the green check mark to insert your BOM into the drawing.

Make Sure Your BOM is Properly Filled Out

You will notice in the example below that all of the fields are not properly filled out. Depending on how your BOM template was created, all of your cells should be populated from the part properties. Of course you can always go back into the original parts and fill out the all of the appropriate Custom Properties, but as of SolidWorks 2008 that is no longer necessary. All of the cells that are linked to the custom properties of a part are now bi-directional. This means that information can be added in either the part file or the BOM and it will be updated in both.

When you double-click on a cell to edit the information you will be prompted with the following alert box. Clicking Keep Link will allow the updates you make to the BOM to also be made to the part file. Clicking the Break Link button will make the changes only to the BOM and any further changes to the property of the part will not be made to the BOM. I highly recommend you select Keep Link since any and all changes made to the part will be be directly reflected in your BOM.

Don’t Know What an Item is?

Sometimes, if you have no properties filled out for an item and you have no item identifiers in the drawing, you may not know what line of the BOM goes to which part. In these cases you can give yourself a little hint as to which item is being referenced by the BOM line. Right-click the row or a cell in the row to view the menu.

In the right-click menu you have the ability to open the referenced part, this command Open also has the file name of the part. Without opening the part you will get a hint as to how to proceed with filling out the row information.

If all steps were followed properly, we have filled out our BOM and the part properties have been updated as well.

Table Cell, Row or Column Toolbars

As of 2008, instead of using the PropertyManager to update the BOM cells, rows or column; a context toolbar is used to update the BOM contents. Click anywhere inside of your BOM you will see the context toolbar.

Adjusting Fonts

By default, the cells in your BOM should be set to Use document font. I always tell my users to make sure that Use document font is enable at all times, not just for BOMs but for notes and dimensions as well, since it allows for font changes to be made globally.

When the Use document font option is enabled, you can globally update the font in the Document Properties. First, click the Options button in your Standard Toolbar.

Then, select Annotations Font -> Tables to access the Choose Font window. Here any adjustments to the font will update all the cells that have been set to Use document font. For those who use it, the Design Checker excels in this area since it checks to make sure that the document fonts match your company standards, but that is a different post.

If you do want to change the font of a cell manually, deselect the Use document font button in the toolbar. The toolbar will expand to include the standard information for adjusting fonts. Be forewarned, any changes you make to the Document Properties will not be made to cells that are next set to Use document font.

Fit Text

One of the new features in SolidWorks 2008 is the addition of the Fit Text tool. Click the Fit Text button overrides the document font for the specified cell and automatically adjusts the font to fit the entire string in the cell.

The text in the cell, rather then getting scaled down, actually gets condensed to fit on one line. Since the Use document font option is overridden the toolbar expands to include the font information.

Adding Equations

On the toolbar you will see a equation symbol. Clicking this symbol opens the Equation toolbar.

In the Equation toolbar you can create simple equations for quantities, create simple conditions statements, even adjust the property a cell or column points references.

Adjust Cell Padding

Cell Padding refers to the space between the border of the cell and text. In the toolbar you can adjust the cell padding of the entire row, column or just cell.

Hide/Show Rows or Columns

In the toolbar, you have the ability to hide or show entire rows or columns.

This tool works much like the Hide/Show Annotations command. When you click the Hide/Show button your mouse pointer will change to indicate that the command is active. Click the rows and/or columns you wish to be hidden, the entire row will be highlighted.

Click the Hide/Show button once again and the selected rows and/or columns will be hidden from view. The items numbers will not be renumbered, instead if you hide a row in the middle of the BOM the item number will be skipped.

To show the hidden rows once again, click the button once more and deselect the rows you wish to be displayed once again.

Group/ungroup selected rows

The Group/ungroup button allows you two group two more more items in the BOM. When items are grouped they share the same item number. To group rows, select two or more rows and the button will become active in the toolbar.

Clicking the Group/ungroup buttons changes the items numbers of the rows to be the same number. To ungroup,  select the rows and click the button once again.

Well that’s it for today, I don’t want your head to explode with too much information in one post. Later this week I will be covering more BOM usage. So until then, Have fun with SolidWorks and as always feel free to contact me with any questions and/or problems you may have.

Creating a BOM from an Existing Template

SolidWorks comes preloaded with some BOM templates that may or may not be sufficient for you company needs.If they works for you, great! That means less work for you  but for the rest who are not as fortunate we will begin with one of these templates. First open an existing assembly drawing or create a new one from an existing assembly.

Next, select Bill of Materials from either the Annotation toolbar or the Shortcut bar.

As you may know you cannot insert a BOM into a drawing without having it associated with an assembly or part. This is why we are using an existing drawing that has an assembly inserted. When prompted select the assembly view in your drawing.

Bill of Materials PropertyManager

When you insert a BOM into a SolidWorks drawing you are presented with a few options that you set in the PropertyManager. Below is an explanation of each:

Table Template

In the Table Template section of the PropertyManager click the Open table template for Bill of Materials button to select the desire BOM template. We will be using this BOM template to build our own BOM.

Table Position

With the Attach to anchor point enabled the table will be attached by the nearest Stationary corner of the table to the anchor point defined in the sheet format.

BOM Type

In the BOM Type section of the PropertyManager select how the BOM will display the components and sub-assemblies of the assembly.

• Top Level Only – Displays only the top level components and sub-assemblies in the BOM. This will most likely be the option you  use the most.
• Parts Only – Displays only components in the BOM. Sub-assemblies will not be displayed but the components of the sub-assemblies will be displayed. This option could be used when you have sub-assemblies used solely to break up the assembly into easily handled sub-assemblies but should not be displayed in the BOM.
• Indented assemblies – Shows the Components and Sub-assemblies of the assembly as well as the components that make up the sub-assemblies. The components will be listed below the appropriate sub-assemblies minus the item number. If it is desired to have an item number listed with the indented components select Show numbering and numbers will be shown based on the parent sub-assembly Item number.

Configurations

Select which configurations will be used to populate the BOM.

Part Configuration Grouping

This section controls the display of part configurations and is not related to the previous Configurations section.

• Display as on item number – When enabled each part configuration in each top-level assembly configuration shares the same item number.
• Display configurations of the same part as separate items – When a component has multiple configurations each configuration is listed separately in the BOM with its own item number.
• Display all configurations of the same part as one item – When a component has multiple configurations the component is only listed once in the BOM.
• Display configurations with the same name as one item – When more then one component has configurations of the same same name they are listed once in the BOM.

Item Numbers

Allows you to set the numbering options of the BOM.

• Start at – Sets the starting item number of the BOM. In most cases this will be set to ’1′
• Increment – when set to one the item numbers increment by one, e.g. 1,2,3,4,5. Set to 5 and the items numbers increment by five, e.g. 1, 5, 10, 15. In my career I have never seen BOMs increment other then by 1 but who’s to say that there aren’t companies that insist on it.
• Do not change item numbers – When enabled even when you reorder your BOM rows the item numbers will not be reordered.

Inserting Default Template into Drawing

After making the desired selections in the PropertyManager, click the green check mark to insert the BOM template into your drawing.

On inserting the BOM into your drawing, you may notice that the configuration name is in the column header along with the QTY.  Depending on your company standards, you may find it necessary to remove the Configuration name from the header. Before 2008 you had to rename the column header, sometimes just removing the period(.) after QTY. In 2008 it so so much easier. In the Document Properties in the Tables menu, select Restrict top level only BOMs to one configuration before inseting the BOM.

Stationary Corner and Anchor Point

Two elements affect the position of the BOM on your drawing, the stationary corner and the anchor point. First, the stationary corner is the corner of the BOM that will be attached to the anchor point. When inserting a BOM into a drawing the corner closest to the anchor point will automatically be selected. If the stationary corner needs to be updated, select the appropriate corner in the Table Position section of the PropertyManager.

The second element is the anchor point. The anchor point is the point on the drawing that the stationary corner of the table will be attached. You can define the anchor point in your drawing templates to ensure that all of the BOMs will be attached. The best way to define the anchor in a drawing is to right-click Bill of Materials Anchor1 in the Sheet Format section of the drawing FeatureManager and select Set Anchor.

Next click the point on your drawing that will be the Anchor Point.

Adjusting the BOM Header

Depending on the location of your BOM, you may find it necessary to adjust the BOM header to either be at the top or bottom of the BOM. In the Bill of Materials Format Toolbar, you can toggle the column header position from top to bottom using the Table Header button. Click the button and header goes to the bottom of the table, click it again and it returns to the top.

Next, adding the BOM Title. At the Top or Bottom of the BOM, depending on what you did in the previous step, you will see two really really small arrows. In the BOM, these little arrows means a section is hidden in the BOM. Clicking these arrows will expand the hidden row displaying the BOM title. Clicking again will hide the title row again.

Updating Custom Properties for Columns

If you are using a particular custom property in your parts and assemblies that you need your BOM to reference, you can update a column to point to that property. First select the entire column by click the lettered column header at the top of the table then click the Equation button.

In the Equation toolbar, select the desired custom property in the Custom fly-out and click the green check mark. The column reference will now be updated.

Adding a New Column

The one thing our new BOM is missing is the Unit of Measurement column. Right-click on a column and select Column Right or Column Left from the Insert fly-out. If the column is not in the right location you can drag in into place.

When the column is inserted, you will be prompted to select the column you wish to insert. Here will will select UNIT OF MEASURE.

Saving the BOM as a Template

Now that we have created our masterpiece we want to save it as one of our templates to be used later. Right-click the cross in the upper-left corner of the BOM and select Save As.

Next, select the location for your BOM template and click Save. You should make sure that the location you choose is also listed in the Folder Locations section of the System Properties.

Well, that concludes our coverage on creating a BOM template. I know it was a long post but there was a lot of information to cover. I will be covering using BOMs next week, so have a great weekend and as always keep those great questions coming.