detailing from .stp files

[ptc-5323661]

I have a doubt that is if we convert .stp file in to .prt file in pro-e........and after that i want to make a drawing of that prt file but i cant call any views,there are only two views standard and default orientation.but iwant to make orthographic views of that part or sub assembly or anything it is.............

Can anyone suggest me an answer

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[ptc-5323661]

if any body didn't understand the question u can ask me back.............because the solution for it is very precious to me

[dschenken]

Look in the help files for Saving Views and Orienting the model.

You can use Google to search for "Pro/ENGINEER Wildfire 3.0 Tips - U of M"

[TomD.inPDX · Accepted solution]

You can also create new views by adding datum planes. You can either create datum planes based on geometry or the default coordinate system. You can also add planes using the import data doctor (edit definition).

once planes are established, you can create views to your heart's content. You can even create those views only in the drawing when you set up the view and not have ot save them in the model, however, that is the easiest way.

[ptc-5323661]

I had created the Planes using the coordinate system and developed the modelling and to set the views in the view manger but i couldn't get the orthographic views.........they are some what inclined

[TomD.inPDX]

Depending on the complexity of the model, specifically if there is no "normal" that is easy to reference, it makes it a bit more challenging, especially if the default coordinate system is not in a usable orientation. It may take some work to get planes where you want them to create views from.

You are using the "SAVE" in the view manager, right? "SET" is used to recall saved views.

If you want to post a picture of the part as it is when imported, maybe we can give better direction.

[ptc-5323661]

Currently i am working on the biw fixtures project..........and the problem raised when going to drawing

[TomD.inPDX]

I do not understand BIW.

What version of software are you using?

Can you add an image?

Do you want to post a file for someone to look at?

If you use the Use advanced editor in the upper right corner, you can attach files.

[dschenken]

BIW = Body In White. From Wikipedia:

Body in white or BIW refers to the stage in automotive design or automobile
manufacturing in which a car body's sheet metal components have been welded

[TomD.inPDX]

Now why couldn't I have figured that out

Thanks!

[Mahesh_Sharma]

Rajanarendra,

You may try below options:

1. Instead of directly opening a step file, create a part and import step in part using Model > Get data > Import > Import Step file. This will provide you all predefined views, whereas directly importing step will not give any views.

2. Directly open the step file > It will import with a coordinate system and Import Feature ID in model tree > Drag "Insert Here" on top of "Import feature ID" > Click on Plane > It will create three datum planes. These planes can be used for View creation as suggested by Antonius.

[JonathanHodgson]

To create an orthographic set of views in the drawing, you only need to orient the first view correctly (which as mentioned can be done in a number of ways).

You can then create projection views from the first view (and from each other) - there is no need to create a named view for every projection.

[TomD.inPDX]

I think the original request is to make the "right" starting plane where the original coordinate system was not oriented in the way they needed it.

Now that I know this is a car body, I can see how one would want to orient the body for fixturing based on a common inspection plane.

So yes, existing geometry can help create the basic 3 planes for the new orientation desired for continued development of fixtures and drawing orientation. physical flat surfaces or points can be used to define the primary plane, and the rest can follow normal from this one plane and a point. The 3rd of course is normal-normal to the 1st 2 and a vertex.