Copy Sketch and Maintain the Sketch Relations

SOLIDWORKS has had, and continues to have all kinds of functionality embedded in the most basic of windows commands – Take the “Copy” command for example.  In this example we will use simple Copy & Paste Functionality to make an exact copy of the sketch and maintain the relations applied to the original.

Copy and Paste Sketch Process

The Basic Workflow to copy the sketch is simple:

1. Select the source Sketch
2. Type CTRL+C as a shortcut for the “Copy” command
3. Select the Plane that will receive the sketch
4. Type CTRL+P as a shortcut fr the “Paste” command

Copy Sketch

As with most things, it turns out there is a little bit more to the story here to be a complete success. Upon pasting the sketch you may discover that the geometry appears Under-defined, which is the spot where most folks give up and turn back.

Copy Sketch Plane is different

The reason the copied sketch becomes under defined is due to the lack of relations that are controlling the location of the sketch with reference to the origin. The original sketch had a coincident relation that held the lower left corner of the sketch on the origin.

Under defined sketch

If you add some dimensions or relations to control the location of the sketch, or simply add a fixed relation – The sketch will then become fully defined and ready for reuse.

Fully defined sketch

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Suppressing SOLIDWORKS Sketch Relations

A neat trick that not many users are aware of is the ability to suppress a sketch relation. While this may not seem like the type of thing that needs to be done very often, it’s very useful when it is needed. When suppressing sketch relations, use the following technique:

1. Go to Display/Delete Relations (on the Sketch tab of the Command Manager)
2. Select the sketch relation from the list on the left
3. Check the box to suppress it
4. Choose which configurations you want it suppressed in (This configuration/All configurations/Specify configurations)

It’s as easy as that. Here’s a screenshot showing you everything you need to know:

 

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Power Trim (3 quick tips you might not know) (video)

 

I bet you use Power Trim on a regular basis. But I ask you this – Do you use it to its fullest? I’ve got three quick tips for you the next time you use Power Trim:

1. That red square that shows up as you click and drag? That’s your undo button! Don’t let go of your left mouse button until you’re comfortable with your trim. if you accidentally trim a little too far, move your mouse back to the red square to undo last and try again!
2. Already knew that one? How about clicking and dragging an entity to extend it? You can also use this click and drag method to separate corners rather than trimming away a whole segment and redrawing.
3. And finally, with Power Trim active, you can left click an entity to trim, and then move your mouse to the location you’d like to trim or extend to and left click again.

 

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Start sketching by selecting an edge

 

This is one of those interesting tricks that can be very useful and you may not be aware of.
Simply select any Edge of any solid body and click INSERT->SKETCH. A sketch plane is created automatically, normal to the edge selected, with the origin coincident to the end point nearest to where the edge was selected.

This operation supports any edge type from linear and prismatic to completely organic and lofted. You could also use INSERT-> Reference Geometry to add a plane perpendicular to a curve, but this takes care of all those steps AND starts a new Sketch.

 

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What is the Vary Sketch Option in a Pattern?

 

I have an option that you might have overlooked or just didn’t know what it does.  It’s the Vary Sketch option.

The definition from the Help File says, “Select the Vary Sketch option to let the pattern instances change dimensions as they repeat.”  Let’s take a look at what you have to do and how it might help you.

So what I’m going to do is create a triangular part first.

Now we need to have a feature added to it.  It can either be a Boss or Cut.  As we pattern the feature, we want it to follow the top angled edge.  The sketch that is used for the feature is important.  First off you want it be fully defined.  This is important so we know which dimension changes.  Next we want the top of our feature sketch to be dimensioned to the angled edge.  This will allow the feature to follow this angle.  If you would add a height dimension, your pattern would not work.

Here comes the unique part.  Start the linear pattern tool.  Choose the feature you want to pattern and set the spacing & instance count.  For the direction, choose the sketch dimension that is in the direction you want to pattern too.  You can always choose a sketch dimension to use it as the direction.  Fun trick isn’t it?

You should have the ability to choose Vary Sketch under the Pattern Options.  If you don’t then it would be a normal pattern that you would expect.

But if you would select Vary Sketch in the options, look at what happens.  It changes the overall height to maintain all the dimension in all the instances.

You might wonder when this option was added to SOLIDWORKS.  I think it was added in the 1997 Plus release.

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Nuggets of Knowledge (video)

3D sketching? Try showing the Sketcher Triad to manipulate geometry in a desired direction (along x, y, z or along a plane for example). While editing your 3D Sketch, right-click in the graphics area and select Show Sketcher Triad.

Need to pick all lines or dimensions but don’t want to turn on your filters? Simply select the desired entity type in the graphics area and use Ctrl+A on your keyboard to pick the rest.

Now that you have all of your lines selected, how about quickly making them construction geometry? Try out Alt+C for this one.

 

 

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How to Modify Sketch

 

SOLIDWORKS has many tools that are often forgotten because they are not on the main toolbars, or talked about much in training classes. One of these tools is the Modify Sketch tool, which has 3 main functions for modifying your Sketch, including Moving/Flipping, Rotating and Scaling.

Modify Sketch can be found in the Tools dropdown, under Sketch Tools, Modify…

To Move a sketch you have two options the first is to enter a Translate value into the dialog box.  The other option is to move a sketch in the graphics area, using the pointer:

• Press the left-mouse button  to move the sketch.
• Point at the end points or center of the black origin to display one of three flip symbols. Right-click to flip the sketch on the X axis, the Y axis, or both.
  •  Flip sketch along X axis
  •  Flip sketch along Y axis
  •  Flip sketch along both axes

To Rotate a sketch you have two options the first is to enter a Rotate value into the dialog box. The other option is to rotate a sketch in the graphics area, using the pointer:

• Press the right-mouse button  to rotate the sketch around the black origin.

Note: The speed you use to rotate determines by how much the angle increments. Slow motion increments the angle one degree at a time; quicker motion increments the angle by ten or more degrees at a time.

• Point at the center point of the black origin to display a point symbol . Click and drag the center of rotation independently of the sketch, then rotate the sketch around the black origin.

Lastly to Scale a sketch select either the Sketch origin or the Movable origin from the Scale About in the dialog box. Once you choose what to Scale About enter a Scale Factor and press enter.

One last item to remember is that you cannot Modify a sketch that has external references, if your sketch has external references you will see the following message and will not be able to access the command until you delete those references.

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Power Trim

Power Trim can be found by clicking on the command “Trim Entities” in the menu bar.

This tool combines trim and extend. Once you’ve selected it, just click and hold down the mouse button, and move the mouse over the lines or sketch entities you want to trim.

If you want to extend a sketch line, just repeat the same procedure, but hold down the SHIFT key, so that “trim” and “extend” can be done in the same command.

The last tip is, if you make a mistake, instead of deleting everything and starting over, just go back to the red square, and your last action will be cancelled.

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Disconnecting One Line from Another Line in a Sketch

Have you ever wanted to disconnect one line from another one in a sketch, eg, at the point indicated in the image below?

Well, it’s possible using either of two little known sketch settings:

1. No Solve Move
2. Detach Segment on Drag

They are shown below.
Once either of these settings is turned on you can drag a line away without the attached lines “following it”.

Unfortunately you can’t drag it from an endpoint, the whole line must be dragged and then the end points re-attached as required.
The video below shows this process in action.
Disconnecting 2 Lines in a Sketch – video
Admittedly, in this simple example, it might have been quicker to simply delete the line in question and draw another one, but I think it’s always nice to know about alternative techniques.

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Special Dimensions

The first of these methods require knowing the correct order and geometry to select to the get the dimension you’re looking for.  I will go over each in detail, and also show the order in which you need to pick the geometry with the Dimension Tool.
Arc Length Dimension

To get the length of an Arc in SOLIDWORKS using Smart Dimension, you need to first select the two end points (1), then select the arc itself (2).  Once you’ve done this you will be presented with a preview of the dimension (3), which you can then place and specify the desired length.  It’s worth mentioning that this dimension by default is a driving dimension.  However, you can add this dimension also as a reference dimension if you only want to see the value.

Angle Dimension without Construction Geometry

The next dimension allows you to create an angle between two endpoints of an arc without the need to create any Construction Lines.  Typically, users spend the extra time to draw Construction Lines from the center of the arc, and then place angular dimensions on those.  To create this dimension, first, like before select the two endpoints (1).  This time however, select the center of the arc (2).  Like before, you will be presented with a preview of the dimension, in this case an angle (3), which again, you can place and use as either a driving or driven dimension.

Angle Mates without Construction Geometry for Lines

Finally, the last type of mate is another Angle Mate, this time specifically for Lines.  Like before, often times you need to have some form of reference or construction geometry available to reference.  However, in SOLIDWORKS 2015, there’s a new way to create these dimensions, and very flexible in how it works.  First, you need to select the line you want to apply the angle to (1).  Then, select one end point of the line (2).  As soon as you do this, SOLIDWORKS will now present you with a reference Compass in which you need to specify which polar direction you want to apply the angle to (3).  Once you do this, like the other two examples, SOLIDWORKS will present you with a preview of the dimension, and you only need to place it (4).  And of course like the other two examples, this dimension is driving by default.

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SolidWorks Numeric Sketch Input Tutorial

Some good simple time savings in this vid.

Solid Professor

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Move Sketches

Moving Sketches while in Edit Sketch mode is not always the easiest task, ESPECIALLY when they are Under Defined Sketches or those that are Copy/Pasted from DraftSight or other 2D applications. 
Where most users run into trouble is that they feel, and I don’t disagree, that you should just be able to window select all the sketch entities and then just grab a point and drag the whole group. While this sounds logical, it has simply never been the case.
Then you could try the Move Entities command, but it doesn’t always snap to the final location as you might expect.
The following technique is completely effective and very easy to do, you just have to know the sequencing of the clicks.
First, Window select the sketch entities you wish to move.
Second, hold the CTRL key on your keyboard then Pick and Drag the selected entities from one of the points in the sketch.

CAREFUL NOW... The trick here is that a CTRL + Pick and Drag in Windows is a Copy... and that is ‘initially true’ here too. Note the Cursor with the little (+) next to it. If you let go of the Left Mouse Button FIRST, you will COPY the Sketch.

Instead, while in the middle of the ‘Copy Sketch’ operation, release the CTRL KEY while still holding your Cursor. The little (+) goes away and the entire operation turns into a MOVE command. Simply snap and release your cursor when your selected point is in the proper location, or snapped to the origin.

In summary, of the thousands of functions in the millions of lines of SolidWorks code, these are some of the more useful yet somewhat hidden functions I use frequently. I hope that you found something you didn’t know about that helps you improve your quality of designs, but most importantly saves you time and effort during your creative process.

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