How to re-orientate an Imported Model
Sometimes when models are imported into SOLIDWORKS from alternate file types, the co-ordinate system can line up differently. Below we can see the before and after of an out of line part and in line part.
In this tutorial we will go through the step by step process of correcting this orientation. This is useful if you are making adjustments to the part, but the main benefit of this is for producing drawings. Without reorientation can be near impossible.
In order to do this, we must create a new co-ordinate system.
- The first step is to identify how you want the model to be presented. In this case we want the front plane to run parallel with the face selected in the image below. Now the face is selected, we will create a sketch on this face.
- To create a co-ordinate system, we will sketch out references. In this example we will create this new system with the origin in the centre of the circular cut out.
- Draw a point in the centre of the circle
- Sketch a line out from this point, creating a perpendicular reference with the edge
- Sketch a second line, perpendicular to the fist line drawn
Note: This can also be created with existing sketches or edges
- Exit the sketch and create a new co-ordinate system through the features tab or – Insert>reference geometry>coordinate system
- We can now use the sketch we have just created as reference. Starting with the point, select this as the origin, then select the lines in a suitable order to define the X,Y,Z direction. These can be flipped to later orient the part how you want.
Now that the new co-ordinate system is in place, we can alter the orientation of the part.
- Go to File>Save As. DO NOT save as a sldprt. Multiple file types work but in this example we will be using .IGES. Select the file type and click Options at the bottom of the save as dialog box
- This opens an additional dialog box. We are only interested in the dropdown menu at the bottom. Select the dropdown and highlight the new co-ordinate system we have just created. Click Ok.
- Save the file and open it up. When selecting viewports the part should now be correctly aligned. This can be seen in the images below for both modelling and drawings.