Why are the default axes of solidworks (orientation) not good?
In front view, we should have the Z axis for altitude. And this is not the case, we have Y.
Can I change this default choice for all new parts or assemblies?
In front view, the Y axis is vertical, the X axis horizontal, and the Z axis goes to the bottom.
I don't understand your question?
If you want, you can create new views but I don't think that's the solution.
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You can create a new Via coordinate system reference geometry. There, we can re-orient by selecting an X, Y and Z axis
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Hello
As for the why, perhaps we should look for the explanation in American standards. It's true that in the European industry, we are more on the Face plan on X-Z.
You can artificially reorient your axes, but you won't be able to have a perfect model:
- You can reorient the views (as proposed by @Bart) and save this new orientation.
- You can rename your reference planes.
- But you won't be able to change the order of the datum planes in the tree.
You will get the attached image.
This operation must be repeated on your models of parts and assemblies.
screenshot2205.jpg
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Thanks for the info, but I think the designers at Solidworks made a big mistake.
Because in all industrial drawing guides, we have Z for the altitude in front view. (see GDI or Fanchon..).
The problem is that I send a step file to my German client (demanding..). He works under catia, and he reproaches me for not putting Z for altitude. I can create a new coordinate system to record as a step. But it's a shame that this is not the original case.
I tried to modify the template files by re-orianting the default views and renaming the planes. But this is not right, because when you make a new sketch the sketched axes that start from the origin (in red) turn upside down. not great.
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[EDIT: redundant message compared to the previous ones that were not displayed when I refreshed the page]
Hello
Yes, you just have to reorient as you want (by putting yourself normally on the top plane), and update the standard views, by clicking on space and clicking on the telescope with a star that corresponds to "update standard views", and choose this view as the front view.
The Z axis is thus directed upwards. You can then rename the planes to suit them.
To do this for all new parts and assemblies, you need to do this for document templates.
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[Edit: on the other hand this solution works]
For this problem, it is enough to register the STEP with a second marker created later, see here:
http://help.solidworks.com/2012/French/SolidWorks/sldworks/t_Creating_a_Coordinate_System.htm
And choose this coordinate system in the STEP export options:
Exit coordinate system. Select a coordinate system for export. If you select -- by default -- no transformation matrix is applied.
Spring:
http://help.solidworks.com/2012/French/SolidWorks/sldworks/HIDD_EXPORT_OPTIONS_STEP.htm
Another solution may be simpler: insert the assembly or part into an assembly, and constrain it to have the right orientation.
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FYI, is it the selected answer that solved the problem or the other one that starts with "[Edit: on the other hand this solution works]"?