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SolidWorks 2010 Rapid Dimension

Adding dimensions to parts on drawings is now quicker in SolidWorks 2010 with the addition of Rapid Dimension. Once the user enters the Dimension command, Rapid Dimension allows the them to quickly position dimensions (almost automatically) as they are added. Not only will dimensions automatically space out correctly as they are inserted, they will be inserted at the correct location, even without that location in view.

Now, each time a dimension is added to a drawing, SolidWorks will pop up with a pie, divided into two pieces for linear dimensions or four pieces for radial dimensions. (Technically, these pies are called the rapid dimension manipulators.)

Linear Dim Pie

Each piece of the pie represents the direction (which side of the part) that the user can choose to place their new dimension. When the user selects the half or quarter, the dimension is placed in the correct location on that side of the part within the drawing view.

Rapid Dimension in Action

Two methods can be used to select the dimension location using the pie. The user can simply LMB click on the portion of the pie in the desired direction. The user can also use a mouseless method, by pressing tab to toggle between the pieces of the pie; then press the spacebar to select. Additionally, the user can choose the ignore the choices offered by the pie to manually place the dimension, just as they would in previous versions of SolidWorks.

The auto-spacing between dimensions is determined by the user’s settings in Tools>Options…>Document Properties>Dimensions within the Offset distances field. The ability to set default dimension line offsets has been in SolidWorks for quite some time, but it’s never been quite so useful as it is in Solidworks 2010.

Offset distances field

Within a few minutes of using Rapid Dimensions, many users will likely become instantly addicted to the new function, as it promises to be a major time saver when detailing drawings in SolidWorks 2010 and beyond.

Deleting Dimensions

One additional item about dimension placement is SolidWorks behavior when a dimension is deleted. If the user deletes a dimension or even just removes text from a dimension, SolidWorks has the ability to automatically realign the spacing of the neighboring dimensions to get rid of gaps caused by that deletion. The user has the option to turn this ability on by going to Tools>Options…>Document Properties>Dimensions to select the Adjust spacing when dimensions are deleted or text is removed checkbox.

Drawings represent final product

One comment I’ve seen about ASME suggests that it is geared towards fully detailing product definition. One trap that rookie designers and engineers will often fall into is over-specifying their parts by placing manufacturing process information on the drawing.

The new designer may do this because maybe a machine shop made the part wrong and was trying to work the rookie’s inexperience to weasel out of their responsibility. Maybe someone in Quality Control was confused by a drawing because they don’t have adequate blueprint reading skills, so they come to the new designer to ask that more information be spelled out on the drawing (when it is already fully specified). These are just a couple of examples. Often, new designers don’t know why manufacturing processes are not included on drawings, nor even that there exists standards that forbid it.

ASME Y14.5-2009 (and previous versions) states:

1.4(d)The drawing should define a part without specifying manufacturing methods. …However, in those instances where manufacturing, processing, quality assurance, or environmental information is essential to the definition of engineering requirements, it shall be specified on the drawing or in a document referenced on the drawing.

It is usually pretty obvious when manufacturing methods are necessary to the engineering requirements, even to the individuals new to the field. Unless one is in particular industries, manufacturing methods are almost never required. A drawing should fully detail the final product without over specification.

ASME Y14.5-2009 adds as an example:

Thus, only the diameter of a hole is given without indicating whether it is to be drilled, reamed, punched, or made by any other operation.

The manufacturer is responsible to provide a final product that complies with the drawing regardless to the processes they use. It is still important for designers to know the processes that will most likely be employed, so they know that the product is economically manufacturable. This does not mean that they should unnecessarily limit the manufacturer to particular processes.

SolidWorks 2010 Usability: Attach Annotations to Dimensions

There are a ton of subtle improvements in SolidWorks 2010 to improve its usability. Many of these improvements might seem small now, but once one is reliant on the new functionality, it will seem like we’ve always had it this way. Attaching annotations to dimensions is now easier with expanded capability. Here’s a couple of examples showing-off these new capabilities.

Drop Annotation Notes into Dimensions

It is now possible to drag an annotation note and drop it onto a dimension, to become apart of that dimension callout. First, LMB click and hold on the annotation note.

Select annotation text

Then, simply drag that annotation note on top of the dimension.

Selected text becomes apart of dimension

The result is that the text from the annotation note is now included within the text of the dimension. One limitation is that the dimension field still does not support borders around selected text.

Attach Annotations to Dimensions

Other types of annotation that can be attached to dimensions include GD&T feature control frames, datum feature symbols and surface finish symbols.

Annotations attach in more ways to dimensions

Annotations and their leaders may now be attached directly to extension lines.
GD&T annotations now may be dropped right into a dimension callout and then detached with the use of the handles in the upper left corner.
Annotations may now be moved around extension lines, and more easily moved from one attachment to another.

SolidWorks 2010: Dimension Palette and Styles

Dimension Palette is a great new function in SolidWorks 2010 that allows the user to edit most commonly accessed aspects of a dimension, right from the main drawing view pane.

Simply highlight or LMB click on a dimension. A ghost image of its Dimension Palette will appear nearby. Move your mouse cursor over the ghost. This forces it to fully materialize. (I’m reminded of Ghostbusters for some reason.)

Dimension Palette

From that point, many of the dimension’s attributes may be directly edited, such as tolerance style and range, dimension accuracy, and tolerance accuracy. Also editable is text above, right, left and below the dimension. Additionally, formatting is editable, including dimension position and justification, reference parenthesis, and inspection obround outline. To aid in use of these new functions, small pop-up hint fields appear as the mouse cursor moves over each element.

Finally, the user can also quickly apply saved Dimension Styles (formerly known as dimension favorites) to the dimension. This can be accessed by clicking on the gold star icon in the upper right of the Dimension Palette. Dimension Styles are much more automated than the old dimension favorites. Not only does the user have access to any saved Styles, SolidWorks will also restore recently used formatting changes as Dimension Styles.

Dimension Styles

This means, when the user makes a change to a dimension, SolidWoks will automatically save the user’s change as a Dimension Style. Automatically saved Dimension Styles will show up in the Recent tab of the Styles window. These Styles only reside in the current drawing. (In order to use these Styles in another drawing, the user will still have to save the Style in the same way dimension favorites have been saved in previous SolidWorks releases.)

To replicate the same changes to multiple dimensions, the user simply has to edit one dimension (preferably through the Dimension Palette). From that point on, to apply those same changes to other dimensions, the user need only select the Dimension Styles button for affected dimension and select their previous change from the Dimension Styles window.

Basically, the user can paint any various dimension formats as Styles to any following dimension. This is a very cleaver execution of a long standing Enhancement Request to allow dimension formatting to be quickly copied from one dimension to another.

Don’t quote me on this, but if I remember correctly, the current limit on the number Dimension Styles stored in the Recent tab is ten. This may change at some point. One added function I’d like to see within the Styles window is the ability to delete Dimension Styles from the Recent tab. As always, with any great new functionality comes even a greater number of new requests for improvement.

Dimensioning of Slots in SOLIDWORKS for ASME Y14.5

This entry is part 4 of 8 in the series Dimensions and Tolerances

Ever since the additions of the slot sketch tool for 2009 and the Hole Wizard Slot for 2014, SOLIDWORKS almost seems like a whole new software for the those who design machined parts. Adding these tools were long overdue. Additionally, SOLIDWORKS supports the standard methods for dimensioning slots when they are created by using these tools.

ASME Y14.5M-1994 paragraph 1.8.10 and figure 1-35 provide three methods for the dimensioning of slots, with no stipulation regarding which is preferred for particular scenarios. (Note: all three methods require the insertion of a non-dimensioned “2X R” note pointing at one of the slot’s end radii.)

In one fashion or another, SOLIDWORKS supports all three methods, though it does have a default for both simple slots and arc slots. For brevity, this article will only cover simple slots.

The first slot dimensioning method (a) provides the width and the distance between the end radii center points.

Dimensioning Method (a)

Method (a)

The second method (b) is the easiest and simplest to dimension. Simply state width and overall length, and use an arrow to point to the slot’s object line. Though originally reserved for punching operations, ASME Y14.5M-1994 (and later versions) allows for the use of this method on any simple slot. When using Hole Callout to dimension a slot in SOLIDWORKS 2009 or later, this is the type of dimension that is inserted.

Dimensioning Method (b)

Method (b)

The third method (c) provides the width and overall length of the slot in linear dimensions. This method is preferred if the slot has positional tolerances that use the boundary method (see ASME Y14.5M-1994 figure 5-47).

Dimensioning Method (c)

Method (c)

For all of the above methods, add the “2X R” separately by using Smart Dimension tool.

Side note: of the three choices, the ASME board almost left out (a) and (b). The original release draft of ASME Y14.5M-(1994) only shows method (c) in figure 1-35.

Virtual Sharps – What do you call them?

What do you call it when you dimension to the intersection of two lines that don’t come to a point? Virtual Sharps?

In the past, I’ve settled on using the phrase “TO V.S.” after dimensions when they attach to virtual sharps. I’ve seen this type of notation used elsewhere. Another abbreviation I’ve come across is TSC, which I assume stands for Theoretical Sharp Corner. I think that might be older terminology.

Personally, I used to prefer the shorter “VS” because it feels like a more commonly understood term. That said, none of this really matters since the standards don’t specify what’s “proper.” For example, ASME Y14.5-2009 uses the term Point Location but doesn’t provide any identification symbols or abbreviations for this concept.

SOLIDWORKS, on the other hand, generously offers a variety of marks to identify virtual sharps. The main problem? These markers are often so small on certain drawing scales or radii that they’re nearly impossible to see without magnification. Another issue is that none of these marks are defined in any standards. And, honestly, a third problem is the hidden nature of the functionality.

You have to know how to create a virtual sharp mark—there’s no dedicated button or icon for it. It’s a short sequence of steps that you’d never guess without guidance. Here’s how it’s done in a drawing:

Select the two object lines that intersect in space.
Use the Point sketch tool.

How is anyone supposed to intuitively figure out that you need to use the Point sketch tool for this? Seriously. But hey, at least SOLIDWORKS provides some method. That’s more than can be said for the standards.

I guess my question is: What are others doing to identify dimensions that reference virtual sharps?

Anyway, here’s an updated article about Virtual Sharps.