how to change default angle of projection in creo drawing

[vdevan]

when ever i create a drawing, the angle of projection is by default is third angle.

Is there a way to have the default angle of projection as First angle..?

Thanks in advance.

[StephenW · Accepted solution]

For a drawing that is already started, you need to go to FILE  - PREPARE - DRAWING PROPERTIES and change the option PROJECTION_TYPE to first_angle.

For new drawings:

If you use a drawing template, you will need to change the drawing template in the same way above and save it.

If you do not use a drawing template, you will need to edit and save your drawing setup file to specify the projection type. You can find your drawing setup file by looking in the config.pro under FILE - OPTIONS - CONFIGURATION EDITOR and find the option that says DRAWING_SETUP_FILE. That option will tell you the path and filename of your drawing setup file. Open that file with a text editor and change PROJECTION_TYPE to first_angle.

[vdevan]

Hi Stephen, 

Thanks for the reply, that method of editing the setup file seems to be working , but does not seems to be the easiest way to change this simple option. ( i do not mean to disrespect your answer, but i blame creo here).

Instead, i would rather use a template and use that template to create the drawing.

i tried to create a Template (using, File > New > Format ) , i was able to change the Unit to mm , but i cannot find the option to change the angle of projection. Could you please help me with that.

(looks like i have been doing it wrong , can you please give a short guide)

Thanks a lot for the help.

[MartinHanak]

Hi,

detail option for setting first angle ... projection_type FIRST_ANGLE

In my case it is available in C:\PTC\Creo2_M070\Creo 2.0\Common Files\M070\creo_standards\draw_standards\din_mm.dtl file.

[dgschaefer]

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@vdevan wrote:

... i tried to create a Template (using, File > New > Format ) ...

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A template and a format are not the same.  A format is primarily the title block and drawings size. A format has no drawing set up file applied to it.

A template is actually a drawing file with special features.  Start by creating a new drawing with no format and no model.  Then, on the tools tab select template from the applications section.  This will put it into template mode.  You can then apply a format, set drawing view placeholders, etc. You can search the help or PTC.com for more info no the special features available in template mod.

Once you are done, save this in your start model / templates folder as that's where Creo looks for them when creating a drawing from a template.