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Using Autotrace
Added in 2008, Autotrace is an often overlooked tool that can provide much help in allowing the designer or engineer to convert his or her ideas into CAD models.
The tool enables the user to bring raster images into SolidWorks and automate the process of creating sketches from the images. This process converts raster edges in a bitmap to vectors through detection algorithms. You can help the process by using high contrast, and high resolution images.
You must first enable Autotrace through TOOLS>ADDINS. Once, it is active, you can create a new sketch and insert an image using the command "Sketch Picture". Sketch Picture in its simplest form, gives you the ability to manually create sketch entities on top of an image that you scale and distort to fit your specifications. Most bitmap images are supported, up to 4096x4096 pixels. A common mistake is to exceed this resolution as SolidWorks resamples your source image by dividing the resolution by two. By exceeding this hard pixel limit by just one pixel, you can inadvertently cut your image quality in half! Supported file types include JPEG, TIFF, BMP, PNG, and more.
With Autotrace active, you will get another level of options beyond "sketch picture" that helps to automate this task. You will want to mask off as much of the image as you can to capture just the relevant data from the image. Next, you will want to tweak the contrast and other image display settings to help filter the portion of the image you want the software to prefer as the subject matter for your selection. You also have a color selection tool at your disposal to help choose just a specific color region. This can be useful to draw outlines around shapes or to pick up black lines from a multi colored background.
Once you run the tool, you will see sketch entities based off of the contrasting color elements in your image, all without any manual input of sketch entities. There is usually a bit of cleanup required. Use the trim tools, in particular "Power Trim" to make the corrections. Autotrace is not intelligent enough to see the context of an image; it only sees the differences in colors, so it does not understand a cat versus a vase. Keep this in mind while you work with it. You will most likely need to edit the output some, this is normal. It should still save you a good deal of time in many situations, especially with more organic details that would require a lot of work with splines.
Hiding and Showing in a Drawing When making drawing views of an assembly, there are times you need/want to remove a part or two from a view for clarity. You have some options in this situation. As with creating a configuration in the assembly and showing it on the drawing view, you could also create a Display State and show that on the drawing. However, you don't have to do either of those options though. Probably the easiest method to remove a part from a view in the drawing is to simply right click, the classic SolidWorks answer, on the part in the view and under the header COMPONENT (part name here) choose the command Show/Hide. This selection will show another menu with a selection of Hide Component. This option will hide that part and that part only. Another option is to press and hold CTRL, select multiple parts, right click, and then select the command. Another way to hide parts while drawing is to right click in the open space of the view, and then choose the selection of Properties under the View header. Inside the View Properties dialog box there will be three tabs. The tabs include: View Properties, Show Hidden Edges, and Hide/Show Components. The Hide/Show Components is the tab that will show a list of any already hidden parts from that view. Click in the selection box if not already selected and start clicking the parts straight from the view that you would like to hide. To update the view so you can dig deeper into the parts click the Apply button and you should notice the parts you have selected will hide. In this same dialog, you may select and press delete, or right click and choose delete from the menu. This does not delete the part from the view. It only removes it from the selections and when you click OK or Apply, the part or parts will appear back in the view.
How to Reuse a Linked Sketch Every so often there is a need to reuse or copy a sketch and keep it linked to the original sketch. SolidWorks calls this a Derived Sketch and when you create a derived sketch it creates a "parent-child" relationship between the original sketch and the newly created sketch. This "parent-child" relationship allows changes made on the original sketch to propagate to the derived sketch. A derived sketch can be used for any type of sketched feature that either adds or removes material. To create a derived sketch, use Ctrl-select to highlight the source or "parent" sketch and the face or plane you want to place the sketch on and then go to Insert, Derived Sketch. Use the Modify Sketch command under Sketch Tools to change the orientation of the derived sketch when it is placed on the desired face or plane. It is possible to break the link between a parent sketch and the derived sketch by right clicking the sketch in the FeatureManager Design Tree and select Underive. If a source sketch is ever deleted, SolidWorks will prompt you to confirm the deletion and will underive the associated child sketches.
Sensors in the Template Do you ever need to find out if there are any interferences in an Assembly? Everyone does! How about merging a few ideas into one. Let's take your Assembly Template and sensors. Inside of your template RMB (right mouse click) on the sensor folder and change the sensor type to "Interference Detection" and specify the whole assembly. Set your properties and poof you will now be alerted if there is any interference in new assemblies you create!
Convert to Inch or not Inch (Metric) Have you ever designed something with the units set to metric, but want to know what an inch converts to for a circle or a line? When you create the dimension just type in 1 and the letters "in" and it will do the conversion for you. How about arithmetic, yep it will do that as well. It works the other way as well, so try typing "mm" when your document is in english units.
With the release of SolidWorks 2013 right around the corner I've been thinking about what was introduced in SolidWorks 2012. Every new release brings brand new functions and tools, plus enhancements to existing commands and features. Here are a couple of my favorites introduced in the current version of SolidWorks:
Feature Freeze
If you work with complex parts with many features or with computationally demanding features such as helix or large patterns, you've experienced the frustration of changing a feature and then having to wait for the feature tree to rebuild. SolidWorks 2012 has a Feature Freeze bar that can help with that. This tool can dramatically reduce rebuild time, particularly in the latter stages of design. This will also help prevent unintentional changes to your part model.
After turning it on under System Options -> General, a yellow bar appears at the top of the Feature Tree. You can drag the Freeze bar to any point in the Feature Tree or right-click on a feature and freeze up to that point in the design. Now, features above the Freeze bar are frozen... you cannot edit them and they are excluded from rebuilds of the model. Frozen features are indicated with a lock icon and gray text. If any changes occur to your model that cause frozen features to go "out of date," they get flagged with the rebuild indicator (traffic light). Updating these features is a right-click option on the Freeze bar, and they are rebuilt and then set back to a frozen state. There is also an option to defer updates to inactive configurations. To get a real sense of the rebuild time savings use Tools -> Feature Statistics both before and after freezing features to measure the difference.
Dimension Doubling
Smart Dimensions in a sketch have some really…..smart, capabilities. One of them is the ability to automatically "double" your parametric dimension value when one of the objects selected is a construction line. This is very handy when dimensioning a sketch that you intend to use with a revolve feature or if you are modeling only "half" a feature with the intention of mirroring it later. For the uninitiated, here's how it works: Within a sketch, activate the Smart Dimension tool. Select a construction line and then select a solid object (line, endpoint, arc center, etc.). Immediately, the preview of the dimension text shows the actual distance between the objects. But wait - don't place the dimension yet. Drag your cursor to the opposite side of the construction line and voila - The dimension value instantly doubles! Place your dimension and when you key in the value you can think in diameters. No more fumbling for a calculator or keying in math operators. SolidWorks 2012 improved this long standing capability by allowing "doubling" mode to persist; double a dimension and all subsequent dimensions are doubled. Previously you had to re-select the construction line for each doubled dimension… very tedious.
Assembly Tips-Folders/Isolate It can be difficult to manage numerous components in the Assembly Feature Tree of a large assembly. Years ago, Folders were introduced to help consolidate and clean up the tree. Folders not only clean up the look of your tree, but they also make it easy to change properties of an entire family of components (e.g. Hide/Show, Suppress/Unsuppress). The process to create a folder is very easy. Add parts to folders by highlighting them individually in the tree or using shift/control select to grab a group and right clicking "Add to New Folder". You can also drag components into existing folders.
One final tip for folders involves using the Isolate function. When Right Clicking a folder, Isolate (the ability to hide everything in an assembly except what is selected) is NOT shown as an option; however, if you multi-select a component, either graphically or from the tree, that is NOT in a folder along with a folder, Isolate will be shown as an option.
Relative to Model Drawing Views You have utilized multi-body part design in SolidWorks, perhaps through weldments, and you are ready to create your drawing. The overall drawing will be easy to create, but how do you detail the individual parts? One way to achieve this might be to create a display state or configuration to hide or suppress the other bodies for each view, but there is a much easier way to get what you need by utilizing the Relative to Model drawing view. Relative To Model might need to be accessed under the Insert/Drawing View pull down as it's not a default on the command manager typically. After you select Relative to Model, you will be asked to select the planar face of a model. Simply bring up the part file of your multibody in another window and select the specific part you want to isolate for the drawing view. You will be prompted to identify the orientation of the part by selecting two faces and identifying them as either: Front, Right, Top, Back, Left or Bottom. Once you check off your selections, you will be instantly transported back to the Drawing to place your view. FINAL TIP: Depending on the complexity of your multi-body part, you may also need to select between the entire part or just the selected bodies to be shown in your drawing view.
Two Unique Uses for the Alt Key (1): You can use the Alt key to select anywhere on a table to move or select the entire table. When not using the Alt key you must select the upper corner of a table to move the table. By holding the Alt key you can pick anywhere on the table to click and drag the table around. This also allows you to bring up the properties for the table in the property manager. This is also a helpful tip when moving views. Instead of selecting the edge of a view to move the view, by holding Alt you can select anywhere to move the view.
Two Unique Uses for the Alt Key (2): The Alt key is also the required key when performing in window smart mates. Instead of using the mate command to make your standard coincident and concentric mates, you can use the ALT key to drag a face or edge onto the edge or face of another part to instantly mate the two components together. For more info on smart mates, search the help for smart mates or come on out to TriMech's Advanced Parts class.
The Weldment Tool: You can move, rotate, or scale an entire sketch. Select the sketch and click "Modify Sketch" (Sketch toolbar) or "Tools, Sketch Tools, Modify". Follow the cursor feedback to rotate with the right mouse button. If you float over the black origin in the sketch you will see a slightly different cursor that will allow you to move and/or rotate with either the left or right cursor button. The ability to mirror becomes available when you float over either the X or Y endpoint of the origin and you will see the "Mirror" command available at that time. There may also be times when you would like to scale a sketch and that is done thru the "Modify Sketch" dialogue box in the Factor area.
Sketch Colors: There are times when for graphical reasons you would like to color an entire sketch. I am not referring to under defined and fully defined type colors, but by right selecting on a sketch and selecting "Sketch Color", you can change the entire sketch color. This is a this is for graphical pirposes only, but it can be helpful to distinguish sketches in a complicated part or as part of a sweep's path or profile...or maybe even during loft creation. So remember to show your sketch and then just right select (which is the answer to a lot of "How do I" type questions) and then select sketch color.
We are interested to hear how you use the ability to change the color of an entire sketch.
The Weldment Tool: For people who frequently design structural components within SolidWorks, the Weldment Tool should be a go-to function for supporting your design. The Weldment Tool has an extensive database full of cross sectional profiles, for beam type structural elements. These 2D profiles can be extruded along a sketch to create three dimensional geometry. This feature acts much like the sweep tool within SolidWorks; however, there are a few distinct differences. First, the Weldment Tool will apply corner treatments such as miter and cope. Another advantage is it will automatically generate a cut list comprised of length, material, and the type of stock the member was made from. This metadata can be applied directly to any drawing made from the Weldment part, thus making documentation simple, fast, and easy.
Copy with Mates: When adding multiple components into an assembly it can be rather tedious to keep inserting components and mating them together; especially if these components are exactly alike. By using Copy with Mates within an assembly you not only copy the part you also copy its mates. This preserves your design intent and speeds up the overall design time. Once the tool is activated and the desired part is selected it is as simple as following the on screen wizard.
Highlighting Changed Dimensions: When opening a drawing, if dimensions have changed since the last time the drawing was saved, the changed dimensions are highlighted. To see changed dimensions, you must first save the part or assembly and the drawing in SolidWorks 2012. After you save the drawing with the changed dimensions, the changed dimensions highlighting is reset.
Easier Hiding/Showing of Components: In 2012, in the graphics area, you can press Tab and Shift + Tab to hide and show components. To hide a component, move the pointer over it and press Tab. To show a component, move the pointer over an area containing a hidden component and press Shift + Tab. You can use these commands regardless of the component's state (resolved, lightweight, SpeedPak, or Quick view). The commands are not available when another command is active.
Working with Hole Wizard in 2012: In SolidWorks 2012, there is a small but welcomed change to the Hole Wizard tool. Previously, after defining the parameters of the hole, you would select the position tab and click on a point to drop a hole into your model. The issue with the previous Wizard was the inability to "wake up" existing points or other geometry for use as a reference for placing the first hole. After placing the first hole on your part, you were forced to deselect the point tool from the toolbar and then move the center point of your hole to the desired location on your part. This was, in many cases, tedious and unnecessary. In SolidWorks 2012, this process has become much easier. After selecting the parameters of the hole to be created and clicking on the position tab, you will first select the face upon which you would like to make a hole. Making this selection simply defines the plane on which your hole will be placed, as opposed to generating the hole. Now that your face has been defined, you can proceed to waking up points or referencing existing model geometry to place your hole in the desired location; right from the start. No more going back a forth, repositioning holes in your parts.
Properly saving an STL file: Most file types do not have options associated with the quality of the file when you save it. This is not the case with .stl files. In SolidWorks, when you select the .stl file extension in the save as type drop down menu, an options tab becomes available. Within this tab you can change the Deviation tolerance and Angle tolerance of the file you are going to save. If you want to see how these two variables affect the part, you can preview it by selecting the preview box in the export options window. You want to ensure that your tolerance is not set too low or you will have faceting and related issues if the file is ever exported to a 3D printer. Extra Tip: Prior to saving your .stl, pan your part off to the side of the screen, and make sure the save as dialog box is not covering the part prior to going into the options tab. This will allow you to see changes made to the part in real time, allowing you to see facets as they are being modified.
Using the sketch mirror tool in SolidWorks: Many users are already familiar with the way to use the mirror sketch tool to mirror item from one side of a line to another. Typically, the user will select the mirror sketch tool first and then in the first field in the sketch property manager select the items he/she wants to mirror, then the user needs to select the second field in the sketch mirror property manager to select the item he/she wants to mirror across. This is easy enough, but a quick shortcut is to preselect the sketch entities including the centerline you wish to mirror across (use CTRL-select or window-select) and then hit the mirror sketch tool after making the selections. The user will notice the mirror sketch property manager will not appear. Instead, the items you selected will instantly mirror across the centerline you selected. This technique will only work if a single centerline is selected. If more than a single centerline or no centerline is selected the mirror sketch dialog will appear with the selected items in the first field of the mirror sketch dialog box and the user will then need to manually input the entity to mirror across.
Understanding the sketch convert entities tool in 2012: When converting entities in 2012, users will notice it behaves slightly differently than in the past. It actually works very similarly to the way the mirror sketch tool behaves as described above. If the user preselects the items before hitting the convert entities command, the convert entities dialog box will NOT appear. Instead, the items that were preselected will automatically be converted! This is actually how the classic convert entities tool used to work. If the user selects the convert entities command before making his/her selections, the convert entities dialog box will appear. The user will then need to select the items to convert. The items will convert to sketch entities after the user hits the green checkbox(enter key).
