why am I getting a bottom view on the top

[Anonymous]

When I do a projected view above the base view it creates a bottom view. 

So, my drawing all have the bottom view above the front view and the top view below the front view.

Am I missing something simple?

[andrew.de.leon · Accepted solution]

Hi Jack,

Sounds like you're wanting to create drawings using the ASME drafting standard instead of the ISO drafting standard. By default, ISO uses 1st angle projection (bottom view above front) and ASME uses 3rd angle projection (bottom view below front) when creating projected and section views.

Unfortunately you can't change the projection angle in existing drawings, it can only be done when creating a new drawing. When creating a new drawing, make sure the Standard property within the CREATE DRAWING dialog is set to ASME. This will also switch the available sheet sizes from A4, A3, A2, etc to A, B, C, etc.

Also, the units of the design sets the new drawing's drafting standard and units. If the design's units are metric (mm, cm, m), the new drawing's drafting standard will be ISO and its units will be millimeters. If the design's units are imperial (in, ft), the new drawing's drafting standard will be ASME and its units will be inches. However, in Preferences (General > Drawings) you can specify the drafting standard and units to force drawings to use one or the other.

Hope this helps.

Thanks,

Andrew

15" Retina MacBook Pro (Late 2013), OS X El Capitan (10.11.3), in Sydney Australia

[Anonymous]

Thanks
This helps a lot

[andrew.de.leon]

Hi Jack,

Great, glad I could help.

Thanks,

Andrew

15" Retina MacBook Pro (Late 2013), OS X El Capitan (10.11.3), in Sydney Australia

[Carl_Portman_ProCAD]

In the UK virtually everyone uses third angle projection with mm and inches are a thing of the past.

We require A3 A2 A1 A0 etc with 3rd Angle views as can be set up in Inventor.

If you want Fusion to be taken seriously sort this out !!

I am a registered trainer with Autodesk for over 20 years  and design for some of the major car companies in the UK !!

[sanjay_jayabal]

Hi Carl,

You can override the default projection type in Preferences > General > Drawing.  Set the standard to ISO and override the projection type from First Angle to Third Angle.  I do agree that the same flexibility will be good to have inside the Drawing environment so existing drawings can be changed.

best regards,

Sanjay Jayabal.

[Carl_Portman_ProCAD]

Hi Sanjay

This has worked ISO standard 3rd Angle Projection good chap !

Now how can I set sketched dimensions to expressions other than making a note of dx number
whilst editing the dimension.

regards Carl

[sanjay_jayabal]

Hi Carl,

Glad that worked for you and sorry for the delayed response.  Regarding your question on using expressions,

1. If the dimension(s) you want to reference in an expression are part of the same sketch, then you can simply select those dimensions while adding your expression.  Example, if you are trying to add a relationship between two dimensions in the same sketch such as "d2 = d1 * 3/4", then you edit d2 (the numerical value), click on d1 (that is, click the numerical value you see visually on the screen) and complete the expression by entering * 3/4.

2. If the dimension(s) you want to reference in an expression are part of some other sketch/feature, then I would recommend you give a meaningful name to the dimension you want to use as a reference before using it.  That way it is easy to remember/find.

3. If there are non-dimensional values that you want to use to drive your design intent (and control it/them from a single location) use the Parameters dialog to create User Parameters and use those in expressions.

Here is a reference to using Parameters that you may find useful - http://fusion360.autodesk.com/learning/learning.html?guid=GUID-76272551-3275-46C4-AE4D-10D58B408C20.

I hope this is what you were looking for.  If not, do clarify.

best regards,

Sanjay Jayabal.