SolidWorks Tutorials for Beginners – First Sketch, part 2
Welcome back to our SolidWorks Tutorials for beginners series. We had many requests for text to accompany our SolidWorks video tutorials, and here I’ve published numerous blog posts in response to this learning need! I’m picking up from where I left off, in my previous SolidWorks tutorial, with the Line Tool. If you haven’t read through Lesson 8 (First Sketch, part 1) or Lesson 9 (Line Tool), I suggest you do that first just to get up to speed.
We have just exited our first sketch by clicking on the check mark in the confirmation corner to save our work. If you started your sketch on the sketch tab, the feature manager design tree will display on the left panel.
But, if you started your sketch on the Features tab, using either of the available sketch-based tools (Extruded Boss/Base and Revolved Boss/Base), then SolidWorks takes you to the feature property manager and prompts you to continue modeling a solid from your sketch.
Here’s the sketch we ended up whilst creating some lines in our previous lesson. We started it from the Features tab, by clicking on the Extruded-Boss/Base command. This feature needs to start with a sketch, so we chose a plane, and created a few lines:
Fig 01 – The simple sketch we created using the line tool.
When we click Accept in the confirmation corner, we exit the sketch and are taken to the property manager for the Extruded Boss command. Here’s what we see:
Fig 02 – Exiting the sketch takes us to the Extruded Boss property manager. We see a preview of our extrusion in the graphic area.
In the graphic area is a preview of our extrusion; if we click accept (the green checkmark) our line will now be extruded to a depth of 10 millimeters to create the solid we see here.
If we cancel out of the extrude property manager by clicking on the red X, we are taken back to our sketch.
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I’ll just tweak a couple lines and then exit the sketch, saving my work by clicking Accept in the confirmation corner. This time when we exit, we’re not taken to the extrusion property manager, but the status bar shows us we are in part editing mode.
This line underneath the last node in the tree is called the Separator. It appears beneath the last element you created. You can drag the separator up and down to hide various elements of your sketch.
Fig 03 – Part editing mode after exiting a sketch.
The node for Sketch 3 has a minus sign next to it; that signifies that it is under-defined. Under-defined means it doesn’t have enough relations or dimensions to prevent it from freely moving. This is necessary for precise modeling and manufacturing.
The sketch appears in gray line. If we select its node in the tree, it will be selected in the graphic area, and appear in orange line (default settings).
Fig 05 – Right-click on the sketch node and select Edit Sketch to return to sketch editing mode.
You can see that you’re back in sketch editing mode right in the status bar:
Fig 06 – Look to the status bar if you’re confused; it’ll tell you what you’re doing and sometimes prompt you for actions.
Let’s create another sketch. Not all of your model has to be in one sketch; in fact, it’s easier and smarter to create discrete sketches. To create a new sketch, right-click on one of the planes (Front, Top, or Right) and select New Sketch.
A new sketch opens, called Sketch 4. It’s got its own node in the design tree, and it’s the active sketch. Under it, as we draw, we can still see Sketch 3, in gray line. We’re not changing Sketch 3 with our new lines; these lines belong to Sketch 4. The status bar tells us we’re editing Sketch 4.
Fig 07 – Sketch 4 appears in blue line on top of Sketch 3, in gray line. The status bar tells us we’re working on Sketch 4.
TIP: You can deselect everything by clicking in blank space in the graphic area.
Right now the graphic area displays both sketches. The active sketch is shown in blue line. Remember, the blue line not only indicates that the sketch is active, but also that it is under-defined. Once it is defined (and still active) the sketch will appear in black line. The non-active sketches are visible and appear in gray line.
If you’d rather not see the non-active sketches in your graphic area, in case it’s cluttered or kind of confusing, you can easily hide them. Right click on the sketch node and click the Show/Hide button; that’s the glasses icon you see below:
Fig 08 – Right click on the sketch node and click Show/Hide.
When the sketch is hidden, it will not appear in the graphic area. A hidden sketch will have a grayed-out icon in the design tree; that’s how you know, at a glance, that it is hidden:
Fig 09 – Sketch 4 is hidden and its icon in the design tree is grayed out.
Sketch 3 is visible; it’s icon appears in color. Both sketches are under-defined, as indicated by the minus symbol. However, if you mouse over Sketch 4, you can see it, in orange line, in the graphic area:
Fig 10 – Mouse over the hidden sketch and it will be highlighted, in orange line, in the graphic area. When you mouse away, it will be hidden again.
Note how the origin point is marked with this icon in the graphic area:
Fig 11 – The origin point is shown in the graphic area.
We can also hide the origin point by right-clicking on its node in the design tree and clicking the Show/Hide button.
The Show/Hide button toggles the visibility of any entity in the design tree, not just sketches. To show the sketch, part, or other element again, just right-click and click on the Show/Hide button again.
We’re finished sketching for now, so let’s turn our sketch into a part. Click the checkmark in the confirmation corner and go to the Features tab, where we’ll activate the Extruded Boss/Base command.
Fig 12 – The Extruded Boss/Base command on the Features tab.
The Extrude property manager opens. To see the design tree again, click on the first tab (the gear icon) above the property manager. We’re prompted to select a plane on which to create the feature cross-section, or select an existing sketch to use for the feature:
Fig 13 – The Extrude property manager prompts us to create or select a sketch.
We can select from the embedded design tree at the top left of the graphic area; click the plus sign beside part 1 to expand the Part 1 tree into its component branches or nodes.
Fig 14 – Select a sketch from the embedded design tree or select right in the graphic area. Click the plus sign next to part 1 to expand the tree.
I’m going to select Sketch 3 and click the green OK checkmark at the top of the property manager, accepting the default parameters for the extrude.
Fig 15 – The boss-extrude property manager, after we’ve selected a sketch to use as the source for the extrusion.
After I click ok, the extrusion appears in the graphic area, and I see the design tree in the left-side panel.
Fig 16 – The new node for our extrusion, Boss-Extrude 1, appears in the design tree.
The boss-extrude has been assigned a name, Boss-Extrude1, in the design tree. Any other extrudes we create will be numbered sequentially and uniquely as 1, 2, 3, 4, etc, even if we delete previous boss-extrudes from our work.
We see Sketch 4 in the design tree, but what has happened to Sketch 3, which we used as the base for our extrusion? If we click the plus sign next to the Boss-Extrude1 icon, we expand the branch, and see that Sketch 3 was consumed by the feature:
Fig 17 – Sketch 3 is consumed by Boss-Extrude1.
Sketch 3 is also hidden, which you can see by the fact that its node is grayed out. But when we mouse over Sketch 3 in the design tree, the sketch profile is highlighted in the graphic area, in a dotted blue line:
Fig 18 – Mouse over hidden Sketch 3 in the design tree and it is highlighted in the graphic area, in dotted blue line.
This concludes part two of this tutorial on SolidWorks, “First Sketch.” See my previous blog entries for the first 9 lessons in this SolidWorks Tutorials for Beginners series. For my SolidWorks video tutorials, please visit the Solidworks tutorials pages on my website, www.video-tutorials.net, and for hundreds of my free tutorials, please visit my youtube channel, at http://www.youtube.com/videotutorials2.