MCADCafe Weekly Review October 19th, 2017

Ahoy matey! Hop on board and take a look at one of the new mate enhancements this year.

Adding mates in SOLIDWORKS has always been, dare I say it, fun! And now with one of the new SOLIDWORKS 2018 enhancements, adding mates has become easier than ever. With this enhancement, we are now capable of hiding faces while adding mates.

There are different ways for us to take advantage of this feature:

  1. While using the Insert Mates tool
  2. While editing our mates
  3. While using the Copy with Mates tool
  4. While using the Replace Mate Entities tool

For this example, I’m going to use the ALT key while using the Insert Mates tool to show this new feature. While adding mates, simply move your cursor over the face you want to temporarily hide and press the ALT key to hide it. This allows you to select obscured faces without having to rotate your model around or manually hiding components before using your mate tool. As seen in the images below, we were able to hide different faces of our model in order to select faces behind them. This allows us to create mates such as the Width mate quickly and easily.

What's New SOLIDWORKS 2018: Temporarily Hiding Faces When Selecting MatesWhat's New SOLIDWORKS 2018: Temporarily Hiding Faces When Selecting MatesWith this new functionality, your productivity will increase and save you time from moving components around. Previously, you would have to rotate or move components around in order to select obscured faces. Or use the Select Other tool, but there was no way to toggle those hidden faces to show. If you accidentally hide a face you didn’t want to hide, you can unhide it by pressing the Shift+ALT keys. And to restore all the hidden faces back onto your model, you simply press the ESC key. This functionality works the same whenever you go back and edit a mate, use the Copy with Mates command, and use the Replace Mated Entities tool.

With the ALT key, it makes it very fast and easy to temporarily hide and show faces while adding mates in your assembly. So the next time you’re creating an assembly, play around with the ALT key while adding mates to see how much more control you have.

For more information, check out our YouTube channel, get a SOLIDWORKS 3D CAD quote or contact us at Hawk Ridge Systems today. And don’t forget to sign up for one of our SOLIDWORKS 2018 Launch Events! Thanks for reading!


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Methods of Synchronization

SOLIDWORKS does not synchronize property values between models and drawings on its own. For example, if a drawing note or field uses the $PRPSHEET method to link to a model property, the value present at the time the drawing is saved is cached inside the drawing.  This is viewable in eDrawings.  If the linked model property is changed while the drawing is closed, the new value will not be viewable in eDrawings.  The eDrawings viewer can only access the properties of the immediate document it is viewing.  To get these model properties to stick in the drawings we either need to make sure we always have the model and drawing open and editable at the same time, or employ an outside method of synchronization.

Properties in PDM

SOLIDWORKS PDM uses variable attributes to map data card variable values to the Custom Properties of our SOLIDWORKS files.  This is a bidirectional link that will write to the file if the card value changes.  You will observe in PDM that edits to card variables with these attribute mappings established require the file be checked out and will increment the version of the file on check in, since those edits are in fact changing the file.  These attribute mappings are where we can establish a link between the model properties and the drawing properties.  Examine our example variable and its attributes.

SOLIDWORKS PDM: Data Management - Methods of Synchronization

You will note that a CustomProperty attribute for all SOLIDWORKS extensions is accompanied by a $PRPSHEET attribute for drawings.  Under very specific conditions these settings will copy the model variable value to the drawing variable, writing it into the drawing’s Custom Property.  This link is global to the variable for your entire vault.  If you require that some drawings do not carry the values of their models this link will not work, and you may need to look at other methods of synchronization, or use another variable.

The specific conditions enabling this synchronization are:

  • The drawing must contain a note linking to the model properties
  • The data card for the model and the drawing must both contain the variable to be linked
  • The drawing must be saved in the proper context

These are some possible contexts for saving or check in your drawing:

  1. Save the drawing from SOLIDWORKS in a vault folder with the PDM add-in enabled
  2. Save the drawing from SOLIDWORKS in a vault folder with the PDM add-in disabled
  3. Save the drawing from SOLIDWORKS outside the vault
  4. Check in the drawing from Explorer

Context #1 is the only one that synchronizes these variable values.  When using the one model to many drawings option where each drawing represents one model configuration scenario #1 will still always synchronize. This is due to the drawing data card only populating the @ tab with one model configuration’s properties.

If one model produces many configurations where a single drawing file uses multiple sheets to show a single configuration per sheet the trick to maintaining proper links is to set each sheet’s properties to look at a specific view.  See the screen capture below.

SOLIDWORKS PDM: Data Management - Methods of Synchronization

The variable mappings inside SOLIDWORKS PDM will not assist in this type of configuration-per-sheet link.  You will notice the drawing data card has a tab for each sheet, but the referenced model’s configuration properties will not appear there.

SOLIDWORKS PDM: Data Management - Methods of Synchronization

Scenarios #2 and #3 will not perform the synchronization.  No amount of rebuilding or saving will match the drawing’s custom property with the model’s custom property.  The drawing may appear correct, since the notes are pulling from the model’s properties directly. But the eDrawings preview may be incorrect if the drawing has not been opened and saved with the new model property value.

SOLIDWORKS PDM: Data Management - Methods of Synchronization

Forcing the Issue Outside PDM

CUSTOMTOOLS Professional is a SOLIDWORKS add-in that provides the synchronization in either direction, from model to drawing, and from drawing to model.  This works independently from your PDM environment, so users will need to follow standard vault editing procedures to ensure write access is available, and enabled.

Videos of this in action can be found on YouTube.

“Copy model property as drawing property”

https://youtu.be/oXyn4_-9ibI

“Get property from parent”

https://youtu.be/u7apKMMz3gk

 

Forcing the Issue Inside PDM

Synchronizing these properties through the data cards in PDM can have some advantages, especially when it comes to searching for those values.  Since the drawing sheet tabs typically contain no data specific to them apart from manual entry a special add-in must be employed to carry out this operation.  The HAWKWARE team created just such a tool, called Sync Card Variables.

You can find more information about it here:

https://www.hawkridgesys.com/products/hawkware/

As well as here:

http://www.hawkwareapps.com/products/hawkware-for-pdm/sync-card-variable/

Since it was developed as a custom Task you can assign it to happen during a workflow transition to ensure that all values are properly synchronized before the files get too far along.

For more information, check out our YouTube channel, get a SOLIDWORKS PDM quote or contact us at Hawk Ridge Systems today. And don’t forget to sign up for one of our SOLIDWORKS 2018 Launch events! Thanks for reading!

What’s New SOLIDWORKS 2018: Bounding Box
October 16, 2017  by Jacob Ames

The bounding box is an indispensable piece of reference geometry in SOLIDWORKS, representing the smallest area or volume in which a design can fit. While available in weldment and sheet metal models for many years, creating a bounding box for a standard part has required convoluted workarounds – until now. New in SOLIDWORKS 2018, bounding boxes can be created for standard parts with just a few clicks, enabling you to quickly find the maximum dimensions of your design and use the automatically-generated file properties as needed. To emphasize the utility of the bounding box, an organic shape will be used.

Figure 1 – Standard SOLIDWORKS Part with Organic Geometry

Finding the maximum extents of the design shown above would be an exceptionally difficult task without the use of a bounding box. To create one, simply navigate to Insert -> Reference Geometry -> Bounding Box in the dropdown menus. In the PropertyManager, you’ll find two methods for creating a bounding box. While both methods result in the creation of a 3D sketch and file properties, Best Fit will generate the absolute smallest box in which the design can fit, regardless of orientation, while the Custom Plane option allows for the selection of a planar element to define one of the directions of the box. Additional options allow for a preview of the bounding box, and inclusion of hidden bodies and/or surfaces.

Once created, the bounding box exists as a feature in the Design Tree, and can be edited, suppressed, or hidden like any traditional feature. As changes are made to the model, the bounding box will update parametrically while preserving the original settings, but beware when using the Custom Plane option, as model changes may result in a missing reference.

Creating a bounding box for a part also generates a number of file properties automatically, which can be linked to drawings, or otherwise used just like manually-added properties. Click File Properties in the standard toolbar, then the Configuration Specific tab to view these new properties, which include the length, width, height, and even volume of the bounding box.

It should be noted that for multibody parts, creating a bounding box using this method will include all bodies (unless hidden). As such, it’s not currently possible to create separate bounding boxes for each body individually using the new Bounding Box command. However, there are multiple workarounds available to accomplish this, including saving the bodies to discrete part files, leveraging configurations/display states to show a single body at a time, or following the established workaround for creating bounding boxes prior to 2018. Please see our video on this workaround for more information.

As seen here, SOLIDWORKS 2018 allows for the creation of a bounding box and file properties for standard parts in just a few clicks, and this capability is just one of many exciting new enhancements this year. Be sure to check out our What’s New series for additional blogs and videos on all the new features included in SOLIDWORKS 2018. For more information, check out our YouTube channel, get a SOLIDWORKS 3D CAD quote or contact us at Hawk Ridge Systems today. And don’t forget to attend one of our SOLIDWORKS 2018 Launch Events! Thanks for reading!


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SOLIDWORKS Composer: Introducing the Animation Library
October 13, 2017  by Scott Woods

If you’re currently using SOLIDWORKS Composer for creating technical documentation and 3D animations then you already know there is no easier tool available for automating the animation process. SOLIDWORKS has now taken this a huge step further by including pre-canned animation templates.

With the new Animation Workshop automatic animation can be easily applied to any part, assembly, or grouping. SOLIDWORKS is once again making life just a little bit easier by automating commonly used actions.

For this blog I am going to be focusing on the new Animation Workshop, located in the Workshops Tab > Publishing > Animation Library. For this entire blog, I will be working in Animation Mode with the Timeline turned on. All settings will be set to default but it is important to note that all properties can be modified before and after the automatic animation is created in order to fully customize the outcome.

The latest enhancement to this Workshop was released with version 2017 SP 3.0.

Currently, there are two animation library groups, Highlight and Motion. The Highlight group controls various properties, such as color, to bring attention to a particular 3D actor. The Motion group adds movement to a 3D actor to show assembly, disassembly, and other movement actions. Under each group, there are several Animation functions. Each highlights or moves the selected model a little differently so play around with them. Also, remember all actions can be adjusted before and after you create the animation directly in the Animation Library Workshop. To edit a Step, click on it and the Create button will change to Update.

These actions not only shave hours off of creating animations but bring the end publication to life, automatically adding clean professional animation movements and highlights that you may not have time to create manually. And why would you want to when it’s automated?

Now let’s apply some animations.  There are quite a few pre-set animations that come with the installation of SOLIDWORKS Composer, here we are going to cover a couple of our favourites using the top cover of this drill press.

The first Animation Library feature on the shortlist is Highlight-Focus. Highlight-Focus creates three seconds of animation, causing the top cover to flash five times and then permanently changes to a darker blue color at the end. By pressing the Create button Composer automatically adjusts the keyframes in the timeline to bring a user’s attention to the part and then applies a color change to prepare the user that an action is about to take place.

Now that the user knows something is going to happen to the cover we are going to apply another automatic animation. This next animation is going to be used to remove the cover and hide it so the user knows they need to remove this part before proceeding to the next step.  For this, we are going to use Motion-RemoveMotion-Remove will cause the part to flash then translate away from the main assembly and then fade away.

Just like that, a disassembly animation of this cover has been created, taking a 20-minute process down to 30 seconds to develop.

For more information, check out our YouTube channel, get a SOLIDWORKS Composer quote or contact us at Hawk Ridge Systems today. Thanks for reading!



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