Hello, this is Kris Lind with Alignex. Have you ever wanted to move the origin within your part model, only to find out it is not possible? In this video, I will be going over two alternatives to doing just that.
The first option I will be discussing, is the use of a reference Coordinate System. Among other uses, this is great option when wanting to export your model with an alternative origin.
We can access the reference Coordinate System through Insert, Reference Geometry and selecting Coordinate System, this can also be found on your Command Manager under the Reference Geometry menu. When the property manager is launched, we are asked to define the origin we would like to use for the new reference Coordinate System, this can be any reference point, sketch point or vertex. For this example, we will create a new reference point. We will select Center of Face, and select the blue face on the bottom of our part. Now pre-selecting the point, we will relaunch the reference coordinate system, define our axis’s and hit ok.
We now see the new coordinate system listed within our feature tree and when looking at our part model we see that the coordinate system is defined at the center of the blue face of the part.
We will now export this part, saving the file as a .step file. Make sure to select the options tab where we are able to select our coordinate system as the output coordinate system of the exported geometry. Go ahead and hit ok and save the part.
When we import our saved .step file back into SOLIDWORKS, we notice that the origin is no longer located at the center of the red face, but it is now defined at the center of the blue face as intended.
If adding a new coordinate system is not an option, and you are looking to relocate the part geometry relative to the origin as well as re-orientate your standard views, the Move/Copy command may be a better option.
Using the reference point we created in option one, we will move the part body, so that the origin is located on the center of the blue face and realign the part, relative to the Global Coordinate System so that our Front View is normal to the blue face as well.
The Move/Copy command can be found under the insert drop down menu, under features. We first want to select the part body we would like to move, under the translate pull down, we will select our reference point, and for the second selection, our origin.
We can now see that our part body has moved and the origin is now located at the center of the blue face of our part. However, when selecting the Front View, we see that the part orientation has not changed and the Z axis is still normal to the Red Face of the part.
In order to align the Z axis normal to the blue face and re-orientate our Front View, we will again use the Move/Copy command.
Once again, we will select our part body, but this time we will use the Rotate pull-down, we will select our origin and input the desired degree of rotation, for this example, I know that to be 255°.
We can now see that the Z axis is now normal to the blue face and when selecting the Front View, we can see that the orientation has been updated.
It should be noted, that the origin of the part is not moving and any feature inserted prior the Move/Copy command will have the origin represented in the original location. We can see this when we show the sketch used to create the Extrude of our bracket.
To find out more ways in which you can save time with your SOLIDWORKS workflows, make sure to subscribe to our Alignex Blog.
Written by Kris Lind
Kris Lind is an Application Engineer at Alignex, Inc. Kris spends his days assisting customers on the Alignex Help Desk and teaching SOLIDWORKS courses. In his spare time, you can find him at the local record store looking thru the used records bins, or outside enjoying a nice hike with his dog.