{"id":1506,"date":"2014-01-15T17:00:21","date_gmt":"2014-01-15T22:00:21","guid":{"rendered":"https:\/\/blogs.solidworks.com\/tech\/?p=1506"},"modified":"2023-09-20T19:05:57","modified_gmt":"2023-09-20T23:05:57","slug":"how-to-change-the-orientation-of-imported-and-existing-solidworks-parts","status":"publish","type":"post","link":"https:\/\/blogs.solidworks.com\/tech\/2014\/01\/how-to-change-the-orientation-of-imported-and-existing-solidworks-parts.html","title":{"rendered":"How to Change the Orientation of Imported and Existing SolidWorks Parts"},"content":{"rendered":"

So today I decided to go back thru and revamp one of my old workarounds for SolidWorks that is still relevant today. The article is based on support calls I have seen over the years and that is how to change the orientation of a part file. I broke this articles in two section because there are different methods, one for Imported Models and another method for Feature Based Models created in SolidWorks.<\/span><\/p>\n

\"Import-1\"<\/a>\u00a0<\/span><\/p>\n

Imported Models<\/span><\/b><\/p>\n

The orientation of Imported Parts when brought into SolidWorks as we all know can be not what is desired for our design intent. When we import those files we are at the mercy of what the \u201cdesigner\u201d in some other CAD Software thought was best for their application. So we can end up with a Front view that is twisted and at some obscure angle or with an Origin that is miles away from the actual part and this can make it difficult to insert into an assembly or create a drawing for the part.<\/span><\/p>\n

\u00a0<\/span><\/p>\n

To correct this is actually a pretty simple process and can be used to cure several problems all at once.<\/span><\/p>\n

First things first correct any problems with the geometry. This means run Import Diagnostics, combine all Solid Bodies, patch all holes in surfaces, etc\u2026.<\/span><\/p>\n

Once you have you model in a \u201cworkable\u201d state you will need to do the following:<\/span><\/p>\n

1.\u00a0Select a face or create a plane that will be one of your 3 Standard Planes and start a new Sketch.<\/span><\/p>\n

2. Generate 2 perpendicular lines in the proper orientation to represent 2 of the parts Axis.<\/span><\/p>\n

\"Import-2\"<\/a><\/p>\n

3. Create a new Coordinate System (Features toolbar, Reference Geometry), use the intersection of the lines as the Origin and the Line for the Axis (X, Y or Z).<\/span><\/p>\n

\"Import-3\"<\/a><\/p>\n

4. Save out the Part as an IGES, STEP, or any other neutral format, making sure one the File of Type is selected to go to the Options.<\/span><\/p>\n

5. In the Options dialog box change the Output coordinate system to your new Coordinate System you created.<\/span><\/p>\n

\"Import-4\"<\/a><\/p>\n

6. Re-import the model back into SolidWorks and it will now be in the orientation of the new Coordinate System and any model changes you made to correct bad geometry should carry over to the new part.<\/span><\/p>\n

\u00a0<\/span><\/p>\n

Existing SolidWorks Part<\/span><\/b><\/p>\n

There are 2 ways to change the orientation of an existing SolidWorks file that is built as a feature based model and both of the methods have their pitfalls. The first method is probably the one with the most potential for failure of other features in the part and that is changing the Sketch plane that the base feature is created on.<\/span><\/p>\n

\"Existing-1\"<\/a>\u00a0<\/span><\/p>\n

The reason this can be bad is because you need to think about the other features in the model and how their Sketches were defined. If they were all defined off of other model faces then everything may work out OK but if anything was based off of a plane it more than likely blow up on you and could cost you a lot of rework time. Also do not forget about the potential issues if you already had a drawing file created for the part as you will have to go in and do some cleanup work on that as well.<\/span><\/p>\n

The second method is a little sounder and that is using the Orientation Dialog Box, this is an alternative version of the View toolbar.<\/span><\/p>\n

\"Existing-2\"<\/a>\u00a0<\/span><\/p>\n

To get to this all you need to do is hit the Space Bar while in SolidWorks, this lists all of the Standard Views and Display Panes. The dialog box has 4 buttons across the top Previous View, New View, Update Standard Views, Reset Standard Views. New View does exactly what it says creates a new view in the exact orientation and zoom of a file, this is a good way to save off obscure views that you may want to put on a drawing or an area of the part that you want to work on later. The Update Standard Views button will allow you to redefine the Standard Views of your part and the way it works is as follows:<\/span><\/p>\n

1.\u00a0Rotate, Zoom, select a face and view Normal To, to get your part in the orientation you want it.<\/span><\/p>\n

2.\u00a0Select the Update Standard Views <\/span><\/p>\n

3.\u00a0Select (single click) on one of the Standard Views listed in the Orientation dialog box and it will now make the Orientation you set in Step 1 to the Standard View.<\/span><\/p>\n

\"Existing-3\"<\/a>\u00a0<\/span><\/p>\n

Just like in the previous method discussed above do not forget about the potential issues if you already had a drawing file created for the part as you will have to go in and do some cleanup work on that as well.<\/span><\/p>\n

\"Existing-4\"<\/a>\u00a0<\/span><\/p>\n

The great thing about the using the Update Stand Views method is that you can always go back to the original view orientation by using the Reset Standard Views button to reset everything back to the way the part was first modeled.<\/span>\u00a0<\/span><\/p>\n

Josh Altergott<\/span><\/p>\n

CATI\u00a0 Support Manager<\/span><\/p>\n

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