Layers have been available for many years in SOLIDWORKS, allowing users to assign drawings entities to them and control many visual aspects including visibility as well as line color, thickness, and style. New in SOLIDWORKS 2018, hatches can be added to layers, providing even greater flexibility when working with cross sections or adding hatches manually. In this article, we’ll cover how to create layers, assign hatches to them, and control hatch color. For added flair, we’ll be working with the deadly, motorized fidget spinner shown below.
Hatches are only available in drawings, and can be manually applied to closed contours/regions or automatically generated by cross section views. A quick cross section of the model shown in Figure 1 results in the drawing view shown below.
Figure 2 – Cross Section of Fidget Spinner Assembly
Before assigning the hatches to layers, the layers must first be created. Click Layer Properties to access the Layers dialog (as this command is not available in the menus or CommandManager by default, use the Search Commands option or enable the Layer toolbar in order to access it). If using a default template, a single FORMAT layer will be shown. Click New to add a new layer, optionally changing the name or adding a description. The remaining column icons can be used to toggle the layer visibility, printing, color, line style, and line thickness, respectively. In this example, 5 additional layers have been created with adjusted colors.
At this point, the hatches can be assigned to the created layers, and will inherit their visibility, print, and color properties (line style/thickness settings do not apply to hatches). Click a hatched region to reveal the Area Hatch/Fill PropertyManager, then (if necessary) click the Apply To dropdown to specify which portion of the view will be assigned to the new layer. Selections include the whole component, the selected region, the entire view, or a single body. Finally, click the Layer dropdown to select a new layer for the hatch. A checkbox under the Options group box can be selected to apply the changes immediately, or cleared to defer the changes until the Apply button is clicked.
Figure 4 – Area Hatch/Fill PropertyManager
If desired, the Material Crosshatch checkbox can be cleared to override the default material hatch pattern and make adjustments as needed. Simply click OK to save all changes. At this point, any further changes to layer properties will be reflected by the hatches assigned to them. If all hatches are added to a single layer, their visibility, print status, or color can be adjusted simultaneously in just a couple clicks.
Figure 5 – Cross Section of Assembly with Colored Layers Applied to Hatches
Layers and colors for hatches are just one of many improvements this year, so 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. Thanks for reading!
Tabs and slots are commonly used to align interlocking sheet metal components, and the new Tab and Slot feature in SOLIDWORKS 2018 allows for corresponding tabs and slots to be created in one operation. This is definitely easier than using a complicated design library feature or separate extrude, cut, and pattern features.
The required selections for the Tab and Slot feature are the edge to add tabs to and the face for the slots. The tabs can be offset from either end of the edge. The spacing can either be set with an equally spaced quantity or spacing length. The length of the tabs needs to be specified and the height of the tabs can be defined with different end conditions. Fillets or chamfers can be added if needed. And the clearance between the tabs and slots can be specified.
Some other notes about the Tab and Slot feature:
Two linked features are created in the FeatureManager Design Tree (one for the tab and one for the slot).
It can be inserted at any position along the slot body.
Groups can be used to manage multiple edges.
It works with planar and cylindrical geometry.
The bodies do not need to be in contact.
It works on regular, non-sheet-metal solid bodies as well.
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:
While using the Insert Mates tool
While editing our mates
While using the Copy with Mates tool
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.
With 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.
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.
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:
Save the drawing from SOLIDWORKS in a vault folder with the PDM add-in enabled
Save the drawing from SOLIDWORKS in a vault folder with the PDM add-in disabled
Save the drawing from SOLIDWORKS outside the vault
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.
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.
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.
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.
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.
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. Thanks for reading!
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-Remove. Motion-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.
Have you ever wanted to create a pattern of an object in an assembly, but also have every instance slightly rotated from the last? In models such as a spiral staircase, it can be time consuming to create all the features separately to achieve one simple task. For example, first a circle would have to be sketched. Then, a Helix and Spiral would be needed to create the curved shape. After that, a Curve Driven Pattern could be used as the final step. Now with SOLIDWORKS 2018, an enhancement to the Linear Pattern feature in assemblies has been created that allows this to be done in one step!
In 2018, when creating a Linear Pattern, you have the option to add a rotation to each instance simply by checking the Rotate instances box. Select your number of instances, rotational reference as well as the increment angle and you can create various patterning possibilities with different outputs. You also have the option to align rotated instances to the seed instance by checking the Align to seed box. This not only will save time in the creation of your design, but also make it easier to modify in the future by not having to adjust multiple features.
Figure 1: Rotated stairs with 20 degree increments
Here are a few examples where I used this new feature in some of my designs. I hope you found this informative. Comment below with ideas for designs you could use this new and cool enhancement on.
Today, we’re going to be diving into a SOLIDWORKS 2018 new enhancement on a widely used SOLIDWORKS feature – Pack and Go! We’ll see how we now have an option to ‘Include suppressed components’ in our Pack and Go in 2018!
First off, what is Pack and Go?
Pack and Go, if you’ve never used it, is a lifesaving feature! It allows you to gather all the referenced files for your drawings or assemblies, and either add them to a specified folder or add them to a zip file!
This is useful for a variety of different situations – some of which are, but not limited to:
Creating copies of whole assemblies, including referenced parts, while being able to append a prefix or suffix to the new files
Sending drawings and assemblies to a vendor or customer, ensuring we grab all the files necessary for vendor or customer to open them!
If you’re interested in learning more about Pack and Go, head over here
Today, we’re going to be diving into a new SOLIDWORKS 2018 sketch enhancement when working with arcs and splines – reverse endpoint tangency! We’ll see the various situations where this new tool can help complete both simple and complex sketches.
Before 2018, when sketching a tangent arc or making two splines tangent to each other – this would happen:
The arc or spline would flip the opposite tangency you were aiming for. Do you remember how you fixed it? Often, I found myself having to delete the arc and spline and recreating them.
Hello (again if this isn’t the first blog you’re reading from me), and welcome to my article on some key enhancements with flattening routes in SOLIDWORKS 2018. In case you aren’t familiar with it, routing is a module that lets you create 3D models of pipe, tube, and electrical routes and is available in SOLIDWORKS Premium. Flattening is the way to represent electrical routes in a 2D fashion for drawings. It’s not this kind of flattening.
I have the routing add-in turned on and I’m working on an electrical harness with a few branches and connectors.
I’ve already used the Flatten Route command and have 2 different styles of flattened routes in the Feature Manager Tree. These are saved as configurations that you can switch to once they are created.
I’m going to start with an annotation flattened view that shows all of the connectors and wires but isn’t to scale. The first enhancement I want to show off is the ability to right-click on a connector or segment and view the connected segment or connector respectively.
This can help you easily identify what goes to where and to make sure things are connected the way you want.
The second enhancement that I’m going to cover is that you can now move around the entire route in its flattened state. To show this, I’ll switch over to the manufacture view in which the harness is to scale and there is a form board outline.
From Figure 8, you can see that the harness isn’t fitting into the outline of the form board. Prior to SOLIDWORKS 2018, to change this you would need to right-click and select Edit Flattened Route to change the X and Y positions. Now, when you right-click you can select the command Move Connected Route Segments.
Once you are in this mode, an XY indicator shows up in the graphics area allowing you to drag the harness to where you want. Alternatively, key in values in the Property Manager.
If you choose to drag it, a ruler shows up that helps you move things a set distance. This is a nice shortcut to help you get things positioned perfectly.