SolidWorks Tutorials for Beginners – The Line Tool
Welcome back. This continues the Video-Tutorials.Net series about SolidWorks Tutorials for Beginners. Please visit our blog archives to view our several previous SolidWorks tutorials about the interface, your first sketch, etc. In this SolidWorks tutorial, we’ll be learning about the line tool. We’ve got an active sketch, and we will begin by selecting the line tool from the command manager.
The Line Tool has a menu flyout from which we can select a Line or a Centerline.
Fig 01 – Sketch 3 is active now. The line tool has a submenu with Line, Centerline.
TIP: A centerline is a line that is construction geometry, meaning it is not used for calculating your model. Centerlines are very useful for helping you create precise, accurate sketches.
With the line tool active, the Insert Line property manager appears on the left side of the screen. The cursor icon has changed also; it is now a pencil with a line symbol underneath it.
By the way, when you activate a command, the left-side panel of the SolidWorks screen switches to the property manager for that tool; that’s the second tab, shown below:
Fig 02 – When you launch a tool, the left-side panel on the screen shows the property manager tab.
To display the Feature Manager Design Tree, click the gear button; that’s the first tab above.
Fig 03 – The Insert Line property manager. The line tool has a unique cursor icon.
The property manager has options for the orientation of the line. By default As sketched is selected, meaning your line will keep the coordinates you select for its start and end points.
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If you select Horizontal you create a horizontal line based on the coordinate position of your first point. If you select Vertical you create a vertical line based on the coordinate position of your first point. If you select Angle you are prompted to enter an angle value to determine the coordinates for the second point.
You can also check For construction under the Options section to designate your line as a construction line, meaning it will not be used in calculating your model. Your line can also be of Infinite length if required; this can be useful for a construction line.
To create a line as sketched, simply left-click in the graphic area to select the first point. You don’t need to hold down the left mouse button, as you do in a graphics program. Once you’ve placed the first point you can continue to move your mouse in any direction, and the cursor displays a preview of the line in what’s known as the “rubber-band” effect, and what’s called “feedback”–that is, you see approximately how long the preview line is, in the current units of measurement you’ve selected.
Fig 04 – The rubberband effect shows us a preview of the line before we click to place the second point, and the preview line length.
The status bar displays the position of the cursor in the two dimensional plane. In my image below, my coordinates are -76.19mm on the x plane and 46.33 mm on the y plane. This means the cursor is 76 mm left of the origin point, and 46 mm above it.
Fig 05 – The status bar when the line tool is active.
The line is zero millimeters in length, since I haven’t placed the second point yet. (I also see that I’m editing sketch 3, and it’s currently , of course, under-defined, which means I haven’t placed any relations or dimensions to “define” the sketch).
Left-click again to finish the line. The start and end points are marked with a blue square while the line tool remains active, and you still see the feedback and rubberband effect.
Fig 06- First line. The tool remains active, displaying feedback and the rubberband effect.
Continue to left-click to create lines, in what’s called a line chain. Each left click is the end point of another line, and also the start point for the next line in the chain. So, these points are coincident because they are shared by two different lines. To stop the chain, double-click. The lines you’ve created appear in blue. The tool remains active, and the property manager remains open.
Any sketch element that’s not defined appears in blue line; once it’s fully defined (with dimensions and relations to define size and position) it appears in black line. These are the default SolidWorks settings, and you can change these if you like on the Options dialog window.
Fig 07 – Our first line chain. Double-click to end the chain. The line tool remains active.
The first and second lines share one coincident point, and the second and third lines share one coincident point. These are relations that SolidWorks has applied for your automatically. SolidWorks also applied parallel relations automatically; this is indicated by the glyph in the green square beside the first and third lines. So, although all we did was activate the line tool and left click a few times in the graphic area, SolidWorks has put in at least four relations for us, automatically.
To keep sketching lines, just left click again in the graphic area. Double click to end the line chain, or you can also right-click and select End-chain:
Fig 08 – The contextual menu when the line tool is active and a line chain is active.
TIP: To create just a single line, left-click to place your first point, and hold the left mouse button down; when you release the mouse button you place your line’s second point.
What if you want to create a line between two points? When I mouse over the end point of this line shown in the image below, an orange circle appears at the end point, and a yellow glyph appears next to the cursor. This is the symbol for a coincident relation, meaning two points that share the same coordinates.
Fig 09- The coincident relation symbol next to the cursor – two concentric yellow circles.
If you left click when this symbol is visible, it means you will place your point coincident to the end point of the line. The coincident relation is applied for you automatically by SolidWorks.
This principle applies throughout the sketch environment: if you left-click to place your point when a relation symbol is visible, SolidWorks will automatically apply it for you, so you don’t have to go back and do it later. This is one aspect of SolidWorks’ built-in intelligence that saves you time and mouse-strokes.
Fig 09 – The rubber band effect, feedback, and another suggested coincident relation.
Now, mouse over to the next point you’d like to connect with your line. When you are there, you will see the coincident relation symbol (the two yellow concentric circles). Click when you see this symbol, and you place the second point of your line coincident to that point–that is, sharing the same coordinates on the sketch plane, or in non-technical speak, in the exact same spot. Again, the coincident relation is automatically applied by SolidWorks.
Instead of left-clicking to accept the coincident relation right now, let’s continue mousing down the line to find out what other relations SolidWorks can offer us.
Fig 10 – The coincident point-line symbol.
The symbol above indicates coincidence between the point and the line. So, if I left click when I see this symbol, I place the end point of my line along the other line; the end point of my line will share a point with the second line. The relation is placed automatically by SolidWorks.
The other symbol you see in the image above is , and this symbol marks the midpoint of the line, or the exact half-way position of the line.
Fig 11 – The midpoint relation glyph.
As I continue to mouse down the line, when I reach the line’s midpoint, or the very center of the line, the relation symbol changes to mark the line’s midpoint: . If I left click at this point, I will place the end point of the line coincident to the midpoint of the second line. So, the end point of my new line, and the center of the other line will have the same coordinates on my plane.
TIP: The use of relations makes your work mathematically precise, which thus reduces the possibility of errors during the modeling, manufacturing or machining processes later on. The fact that SolidWorks often applies them for you automatically makes your work that much easier.
In the status bar, we can see the coordinates of this point: 45.11mm in the positive X direction, and 16.6mm in the positive Y direction, so a little bit to the right and above the origin point of 0,0 (zero, zero).
Fig 13 – The status bar shows us the coordinates of the line’s midpoint.
This panel displays any existing relations between this line and another line, tells me that the line is underdefined, and gives me the option to place relations between this line and another line. SolidWorks automatically assesses which relationships are possible based on the existing entities in the graphic area, and gives me the possible relations under Add Relations. Right now I can apply a Horizontal relation, a Vertical relation, or a Fix relation.
A horizontal relation makes the Y coordinates of the two line points the same. A vertical relation makes the the X coordinates of the two line points the same. A fix relation means you can’t move the line later on by grabbing and dragging; both of its points will be “fixed” in space.
To delete a line, select it with a left click in the graphic area and press delete on your keyboard. You can’t delete a line from the design tree. While the sketch has its own node, each sketch element (line, circle, rectangle) doesn’t get its own branch in the design tree, so you can’t uncollapse a sketch into its component geometric entities.
You can exit the line tool in a few different ways. One way is to click the green checkmark at the top of the property manager:
Fig 15 – Click OK (the green checkmark) to accept your work and exit the line tool.
If you click the red X, you exit the tool without saving your work. You can also exit the line tool simply by right-clicking in the graphic area and choosing Select from the contextual menu:
This is generally the fastest way to exit the line tool, but you will exit the line tool automatically if you activate another tool, like the rectangle tool or circle tool, from the command manager. You can also exit the line tool simply by exiting the sketch (clicking accept or discard in the confirmation corner); this automatically closes the line tool.
After you exit the line tool, you still need to exit the sketch. To save your work, click Accept in the confirmation corner, and to discard your work, click the red X to exit the sketch without saving.
Fig 17 – The Accept & Exit button in the confirmation corner, highlighted when you mouse over it. Click to save your work and exit the sketch.
This concludes our lesson about working with the line tool, and this chapter of our SolidWorks tutorials for beginners series.