Drawing Archives - Page 21 of 29

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.

SpacePilot PRO 3D Mouse: New Software Updates

3Dconnexion recently announced another free software update for the new SpacePilot PRO 3D mouse. The most visible portions of this upgrade include new functions called Model Properties Applet and Intelligent Function Key Notification. Both of these new functions add functionality to the SpacePilot PRO’s LCD. If there ever was a device feature that needs added functionality, it is the LCD on the SpacePilot PRO.

Model Properties Applet

This new applet enables engineers to quickly view supposed key model information on the SpacePilot PRO’s LCD. The claim from 3DConnexion is that this somehow increases productivity and makes things easier for workgroups to collaborate. I’m not sure how this applet makes collaboration easier. The applet just displays fundamental document information on the LCD. It doesn’t transmit this data or pull information from my PDM.

For a drawing, the function is very basic, indeed. The applet tells me that I am looking at a drawing (go figure), and shows the computer network name of the drawing’s author, file size, file creation date, file last saved date, and the computer network name of the last person to save the file. There is nothing particularly “key” or “vital” about any this information. The applet would be far more useful if it allowed the user to modify the information on the display. For example, for me key information from a drawing would be a list of particular custom property names and their values, and the name of the model in the dominant pre-defined view (the view from which the part custom property values are derived).

Slightly more useful information is available for models, including mass, volume, material and density. This same information is displayed for assemblies, though I’m not sure why. Wouldn’t it be more useful to show me the total number of parts in the assembly, or an estimate on how many seconds would be required for a force rebuild (CTRL-Q)? My suggestion to 3DConnexion is to completely dump the file information and add these kind of data for all document types.

Intelligent Function Key Notification

This is a fancy name for the fact that the LCD now displays a quick pop-up window which shows the user which button command they activated. It does this regardless to the applet that is running on the LCD. This way, the user will always have visual confirmation as to which command they just executed. This is a moderately useful function for someone who has just finish mapping their programmable buttons and needs queues to help reinforce the memorization of that mapping. If the user has already memorized their button mapping, this function provides little benefit. For now, I like this function, but I can easily imagine that I will ignore it eventually.

“S” Shortcut key

One bonus for SolidWorks users is that 3DConnexion recently added support for the “S” shortcut key. It can now be added to the programmable buttons directly without having to create a device macro. This function was secretly added to the previous software upgrade for the SpacePilot PRO, but 3DConnexion is now bragging about it. They also stated that this “S” shortcut key support has been added for SpaceExplorer and SpacePilot Speed Keys. My only criticism here is that any key and key-combination should already be supported by the software for these devices. My 1990’s programmable keyboard supports any key combination in its “PF” keys. Why are these not fully supported by 3DConnexion’s 21^STCentury product offerings?

Installation

Having just recently updated my SpacePilot PRO drivers and software with this new announced version, I can say that installation was easier this time around. In the past, installation has been a bit of a pain. One problem plaguing the SpacePilot PRO is that its software and drivers need to be the last item installed on your computer. This means that if any supported application is installed after the SpacePilot PRO software, the SpacePilot PRO software needs to be reinstalled afterwards. Crazy, huh? Anyway, this upgrade was pretty painless this time, and I didn’t even lose my programmable key mappings, unlike previous upgrades and re-installs. New 3DConnexion 3D mice shipped in September 2009 will have the new version of the software and drivers included. Otherwise, for Windows, download them from this location here.

Dimensional limits related to an origin

In SolidWorks 2007 drawing mode, the ability to change the size of individual dimension arrows (so that they were different than the drawing) was limited to a tricky use of favorites. Starting with SolidWorks 2008, that situation improved. SolidWorks now allows the user to set the size for individual dimension arrows. For me, using arrows of a different size from the drawing default was only required once in the past. However, I recently had the need to use this function for dimensioning limits from an origin. This is a special kind of dimension where the tolerance of a dimension is set between two features but applied in only one direction.

From paragraph 2.6.1 of the ASME Y14.5M-1994 standard:

In certain cases, it is necessary to indicate that a dimension between two features shall originate from one of these features and not the other. The high points of the surface indicated as the origin define a plane for measurement. The dimensions related to the origin are taken from the plane or axis and define a zone within which other features must lie.

The origin of such a dimension is shown by replacing that arrow with a circle.

Meaning

This is where we get back to talking about SolidWorks. You can change the shape and size of the arrows on one or both sides of a dimension. The problem is that once the dimension arrow is changed to a circle, its size cannot be adjusted. This means that if the circle is too small (as it likely will be) the size must be changed to the arrow before switching it to a circle.

The following are the basic steps to establishing a dimensional limit related to an origin on a drawing in SolidWorks 2008 or higher.

Instructions 1 and 2

This following chart will then pop up at that location on your drawing view.

Pop up chart

3. Select Size, to bring up the next window.

Arrow size changing window

4. Deselect Use document arrow size and edit the arrow width. Accept by choosing the OK button.

Enter width

No, you aren’t done yet. There’s more. Remember, earlier I said the situation was easier. I didn’t say it was easy.

More steps

Again Again

7. Select the fifth item down on the pop up chart, which is the circle at the end of the dimension line.

Final Product

After all of this, you’ll finally have a dimension that establishes its tolerance from an origin per ASME Y14.5-1994 paragraph 2.6.1 and figure 2-5.

UPDATE: Newer releases of SOLIDWORKS will allow you to apply a size directly to the circle arrow. So, although the above instructions still will work, there are some extra steps that are no longer necessary.

It’s All Over!

When “All Over” is applied to a Profile of a Surface, it pretty much defines the entire shape of a part in every direction.

ASME Y14.5M-2009 has been out for a little while now (after almost a year’s delay). There are significant improvements and clarifications. One addition in particular caught my attention, the ALL OVER symbol. When applied to a Profile of a Surface, it pretty much defines the entire shape of a part in every direction (not just ALL AROUND which applies to the profile of a surface along a particular plane).

The symbol is either a double circle at the vertex of the associated bent leader, or the words ALL OVER placed immediately below the feature control frame.

The symbol indicates that a profile tolerance or other specification shall apply all over the three-dimensional profile of a part. It is applied as “unless otherwise specified” to allow for other existing dimensions and tolerances to take precedence.

The advantage of using this symbol is that it provides control of surfaces over an entire part without regard to part orientation, thus allowing us to directly reference the CAD model as basic and fully controlled, while still detailing critical dimensions and tolerances. This may help companies better parts where they rely on the CAD model to provide complete specification. In fact, where a CAD model is declared basic, companies may be able to effectively place the Profile of a Surface FCF with the ALL OVER symbol right into their drawing title blocks along side other tolerancing information.

Dimensioning of Slots in SOLIDWORKS for ASME Y14.5

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.

Using Empty Views (Part 2: How to use them)

My articles on Empty Views in SolidWorks have been long in coming. This is not due to the topic being complex or anything. It’s just taken me that long to get around to this series. (There’s been a lot of other stuff to talk about in the meantime, such as SolidWorks World 2009, something called a 3D mouse, and rants about this or that.) The Part 1 article in this series discussed how to make, place and size Empty Views. Part 2 now discusses how to use them once they are created.

Use Empty Views as quick Zoom to selection locations

OK, let’s say that one empty view each represents the title block, revision block and drawing notes. How does one quickly move about the drawing to view these areas? There are several methods available in SolidWorks. The following method is likely less common, but is perhaps quicker can more common methods.

First, assign a shortcut to Zoom to selection function. Zoom to selection is found under View pulldown>Modify>Zoom to selection.

Zoom to selection location

To add the shortcut (for much quicker access to this function), goto Tools pulldown>Customize…>Keyboard tab> and then search for “zoom to selection”. From there, simply add a keystroke as the shortcut for Zoom to selection and choose OK to save.

Now here is how to use this shortcut with Empty Views. With the drawing open and with no views selected, look over in the FeatureManager. Select any one of the Empty Views (or any view for that matter).

FeatureManager display of views

As this point, simply hit your shortcut keystroke for Zoom to selection. The viewport will immediately zoom to the area identified by the Empty View.

Zoom to selection of empty view

Choose another view from the FeatureManager and hit your shortcut for Zoom to section again. Each time, the viewport will immediately zoom to the area defined by the selected view.

Using Empty Views for PDF bookmarking

As an added bonus, any views created on the drawing (including Empty Views) will become bookmarks if you save that drawing as a PDF. This adds greatly to the navigability of PDF files for everyone who uses them. Within PDF Reader, the bookmarks will appear to the left (similar to the FeatureManager in SolidWorks). Simply LMB click on the desired view, and PDF Reader will jump to that location.

There are some pitfalls with saving a drawing as PDF, so if your company is experiencing those, then it is not recommended that drawings be saved as PDF. In those cases, print to PDF works better. Unfortunately, bookmarks are not created when printing a drawing to PDF.

Conclusion

The one thing that frustrates me about SolidWorks Empty Views is that SolidWorks Corp reduced their functionality (as discussed in Part 2). However, with a simple hack, they can be used as drawing bookmarks, to contain drawing notes, and to add functionality to PDF files. Additionally, they are always useful for containing sketches, as noted in Part 1 of this series.