Imported DWG files are rotated 90°

[dpoolECL43]

Is the right plane in inventor parts rotated 90 degrees? I've noticed that when I start a sketch on the YZ (right) plane that I'm always started out rotated 90 degrees. If I want to constrain a line horizontally, I have to pick the vertical constraint and vice/versa. This has never been a major issue until today when I tried to insert an Autocad DWG into an existing part. This is a side view of a piece of equipment and when It is imported, it is aligned vertically instead of horizontally. Is there anyway to get this imported DWG rotated correctly without having to modify the DWG? I've imported top views into inventor dozens of times and never had this problem.

These belt guides and pulleys should be aligned with the basin.

[johnsonshiue]

Hi! This might be related to the template you are using. Could you share an example here?

Many thanks!

[dpoolECL43]

The template is attached. I'm just using the Standard.ipt template that shipped with Inventor 2019. I just installed this version, so I'm 99.99% sure this is untouched. I just realized shortly after attaching this that when you create a sketch by selecting the YZ plane of the part origin, the X axis of the sketch points in the same direction of the Y axis of the part origin. I've dug around in these forums and see that people have been complaining about this for years. Is this going to be fixed? It's highly annoying and counter-intuitive. You can see that the axes are rotated by right clicking on the sketch in the browser and selecting "Edit Coordinate System."

This "Edit Coordinate System" functionality, as it turns out, is the solution to my issue. But really it's more of a workaround than a solution since this is obviously broken functionality. I can think of no reason whatsoever that you would want the X axis pointing up; especially since vertical and horizontal constraints are linked to the Y and X axes, respectively. X is never in any mathematical or cad realm vertical.

[johnsonshiue]

Hi! I think I know the issue you are talking about. This is about the way Inventor chooses default sketch coordinate system based on the selected plane. Internally, it has certain rules to pick out the coordinates, which cannot be controlled by the users. As a result, the behavior can be unpredictable. We are indeed investigating a solution to make is more reasonable and intuitive but the solution is not yet available in public releases.

If you want persistent XY orientation, I would suggest you use UCS so that the XY plane is always parallel to the designated plane and the orientation is always Y pointing up and X pointing right.

Many thanks!

[dpoolECL43]

Nope.

1. I place a UCS from the Work Features panel in the 3d Model tab of the ribbon.
2. Put it in some arbitrary place in 3d space and right click to finish the operation.
3. Start a 2d Sketch.
4. Expand UCS 1 in the Browser and pick UCS 1: YZ Plane as my sketch plane.
5. Draw a rectangle
6. Click Finish Sketch in the ribbon.
7. In the Browser right click Sketch1 and choose Edit Coordinate System
8. The Y axis of the sketch is aligned with the Z axis of the UCS. The X axis is pointing up - aligned once again with the Y axis.

Attached here is what I'm seeing in my viewport. It's a little hard to read since the drawing axis is centered on the UCS but if you look carefully, the smaller green Y of the drawing coordinate system is in line with the larger blue Z of the UCS and the smaller red X is aligned with the larger Y of the UCS. Are you saying that I have to change the orientation of the UCS?

[johnsonshiue · Accepted solution]

Hi! I think you misunderstood my suggestion. The workflow I was proposing is to essentially align UCS XY plane to origin YZ plane. Then create a sketch based on the UCS XY plane. In this way, you always have Y pointing up and X pointing right.

If you align UCS to origin totally, the behavior would be the same as on origin planes.

Many thanks!

[dpoolECL43]

Understood. Still a work around, but at least I don't have to repeat the process for every drawing I do. Just one time for the whole part.