Creating curves through reference points or XYZ points

1. How to use curves through reference points in SolidWorks

Feature detail:

Creates a curve through points located on one or more planes.
 
Step-by-Step use:

Create a sketch to provide reference points (here, a circle)
 
Note: Edit the sketch using “construction geometry”
 
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Go to sketch -> circular sketch pattern
 
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Select entities to pattern as the construction line from center to the circumference.

 
Input the number of entities required.
 
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Now, that we have created reference points in a single plane, to create a 3-D sketch let’s create another plane.

 
Go to reference geometry-> plane.
 
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Create a plane parallel to the top plane
 

Tip: SolidWorks is one of the leading designing software because of its user friendly features, while creating reference plane, you can just drag the plane while holding control key , and a reference plane will be created parallel to the plane which was dragged.

 

To project the original sketch onto this created reference plane, go to derived sketch and select the sketch.

 

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To use ‘curve through reference points’ feature in SolidWorks,
 
Go to features-> curves-> curve through reference points.
 
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Select different points, these will act as reference points for the new curve.
 
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Select all the required points to create a closed curve.
 
This feature is mostly used to sweep a sketch through a curve.
 

For example, while modelling the base for a center table. We can sweep a circle through this curve.

 
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Application of ‘curve through reference points’

     

    2. Creating curve through XYZ points:

Feature detail: creates a curve from a list of X,Y, Z coordinates for points.
 
TIPS when using SolidWorks (2010-2015):
 
Tips for working with this tool:
 

Open an existing curve file. Click Browse and navigate to a curve file to open. You can open .sldcrv files or .txt files that use the same format as .sldcrv files. You can also create 3D curves in Microsoft Excel for example, save them as .txt files, then open them in SolidWorks. Create a file containing coordinate values for curve points using a text editor or worksheet application. The file format must be a three-column, tab, or space-delimited list of only X, Y, and Z coordinates. Do not include any column headings, such as X, Y, and Z or other extraneous data.

 

Change coordinates. Double-click in a cell and enter a new value. (As you enter values, notice the preview of the curve is displayed in the graphics area.)

 

Add a row. Double-click in a cell in the row below the last numbered row.

 

Insert a row. Select a number under Point, and then click Insert. A new row is inserted above the selected row.

 

Delete a row. Select a number under Point, and then press the Delete key.

 

Save the curve file. Click Save or Save As, navigate to the desired location, and specify the filename. If you do not specify an extension, the SolidWorks application adds the extension .sldcrv.

 
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This is a step by step tutorial to create an airfoil.
 

Airfoil has standard measurements which can be obtained from the internet. These measurements are nothing but X,Y,Z coordinates.

Download these coordinates as .DAT file.

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Go to .dat extension, right click on it, and click save link as.

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Open these coordinates using Microsoft excel.
 
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These coordinates will look like:
 
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These are standard coordinates, do not alter them, delete first 3 cells. And enter the value ‘0’ to all cells in 3 columns.

 

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In excel, go to file menu, click on save as, set the following parameters and save it.
 
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This saved file is now ready to be imported to SolidWorks.
 
Go to features-> curve-> curve through XYZ points.
 
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This menu will pop up, go to browse and select the coordinate file.
 
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Coordinates will automatically show up.
 
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Click OK.
 
This curve will be formed.
 
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Extrude it to get an airfoil.
 
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