Drawing Archives - Page 20 of 29

SolidWorks 2010 Borders within Annotations

SolidWorks move towards quality has affected many areas in SolidWorks 2010, including annotation functionality. One of particular note is the fact that borders around text can now be added within an annotation note!

The following example has borders added to text using only this new method. No <> tag symbols where used:

Access to this functionality is in the same place as before, under the Border heading within the Note PropertyManager. The only difference is that the border selection now responds to highlighted text within the affected Note. In fact, it only responds to highlighted text now.

Because of this new functionality, some behavior has changed with making flagnotes. As of Beta 2, notice that they will no longer directly attach to a leader unless they are round (Circle border). Some may like this, others may not. Another behavior that might need to be taken into consideration when using these borders is that spacing between lines may be affected, as also shown in the example. Also, this functionality is not supported within dimension callouts.

SolidWorks 2010: Minor tweaks I

One of the funny little things that SolidWorks used to do is that when one added a center mark to a hole (or set of holes) that are already dimensioned, it would not adjust the dimension extension lines to fit with the center mark.

In the march to quality improvements, SolidWorks has fixed this little oversight. Now, when one adds a center mark to a previously dimensioned hole, a gap appears between the center mark and the dimension’s extension line. The same is also true if one adds a dimension to a hole that already has a center mark. No more dragging extension lines after the fact.

Here’s the sample image from the What’s New file:

Woohoo!

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: Mouse Gestures

SolidWorks Corp has been working hard to improve the user experience. SolidWorks 2010 has examples have several innovative interface additions. The one addition that is sure to get a lot of attention is Mouse Gestures.

Mouse Gestures is a simple a menu scheme that is controlled by the RMB and a gesture (or short movement) of the mouse. When the RMB is clicked and held briefly in addition to a very slight movement of the mouse, a wheel menu appears around the cursor location.

Simply continue to hold the RMB down and move the cursor over the desired command. Without any further action, that command will execute and the menu wheel will disappear. If the RMB is released before a selection is made, the menu wheel is cancelled without any command executed.

If the traditional RMB is desired instead of the menu wheel, simply give the RMB a quick click (same as it ever was) without a mouse movement.

As with the “S” key shortcut menu scheme, Mouse Gestures menu wheel is customizable and context sensitive. The user is allowed 4 or 8 gestures with four different menus for each of the major modes: Part, Assembly, Drawing and Sketch. These are customized under a new tab in the good ol’ Tools>Customize… window.

Here are the eight gesture choices that can be assigned to particular commands:

Mouse Gestures is suprizingly easy to use. It’s intuitive when it is activated intentionally. However, I have found myself activating it unintentionally once in awhile. This may result in the surprize command being executed before I even know what hit me. So, for now and for me, Mouse Gesturing will be limited to View Modify functions. I certainly won’t be placing the Quit in my menu wheel. That said, the usual result of the accidental activation is just that the user will see the menu wheel briefly ghost in and out before any command is executed.

Mouse Gestures is a great new tool that looks to be a major time saver for frequently used commands. I’m looking forward to having a bit of fun playing with Mouse Gestures and customizing its functions until I find just the right combination of commands for each mode.

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.