DRAWING CREATION OUTLINE
Do not Rename Parts
After They are in a Drawing
1) SETUP
While you are still in the Part or
Assembly
Mode:
- Create or identify at least one orthographic
view to use for your "Front View"
- Create a good Isometric (3-D) view if needed
- Create your Planar or Offset Section Views
2) START THE DRAWING FILE
- Create a drawing file and give it a name -File->New->Drawing
(usually as the same name as the part or assembly)
- Specify the model or assembly for drawing (if
needed)
- Specify: Empty With Format
- Select (Browse) > Select the ME101_format.frm
(Inch or Metric) > Open
- Done
3) PLACE ORTHOGRAPHIC VIEWS AND
SET SHEET SCALE ()
- Place first general view - Insert Pulldown
->Drawing Views->General
(or
)
- Place (Left-Click in the Graphics Area) and
Orient
the view
to an orthographic view - In the Orientation Box->Saved
Views->Select
a View->Set->OK
- Select View Display
- Select Display Style > Hidden ()
- Select Tangend Edges Display > None
- Apply
> Close
- Project other orthographic views
- Select the first Orthographic
Veiw>Right-Drag to Insert Projection
View
- Drag
the New Views
to the Desired Locations - Unlock the Views if Necesarry
by Un-Selecting the Lock View Position Icon:
- Select the new views (Hold down the Control Key to select
multiple views)
- Right-Click > Properties - The Drawing View Dialogue Box Opens
- Set the View Display to be the same as the first orthographic view
- Scale Sheet to proper size
- Double-Click
on Small Scale Display in Lower Left of Drawing and Enter a Desired
Sheet Scale(Scale is usually between .5
and 1)
4) PLACE THE ISOMETRIC VIEW
- Place isometric (3-D) view Insert Pulldown
->
Drawing
Views(or
)
- Place the view in the desired location - The Drawing View
Dialogue Box Opens
- Select Custom Scale and enter a separate scale for the view if
necesary
- Set the Display Mode for the Isometric View to No Hidden (Not
Follow Environment) >
Apply > Close
- Move views into place - Make Sure the View Lock
is
Unlocked:
-> Select the Views to be Moved and Drag Them Into Place
5) SHOW, CREATE & CLEAN UP
AXIS AND
DIMENSIONS
- Show Existing Centerlines(Axis) from model - View
Pulldown
->Show and Erase (or
)->Show->Axis ->Show All
- Erase Unwanted Axis displays as needed - Right-Click Unwanted
Axis > Erase
- Show Existing Dimensions from model using the
same procedure as above but for dimensions
- Erase Unwanted Dimensions - Right-Click Unwanted Dimensions >
Erase
- Create Dimensions (if necessary) - Insert
Pulldown->Dimension->New
References(or
)
6) CLEAN UP/MANIPULATE DIMENSIONS
- Move Dimension - Select the
Dimension,
and Drag
it to the Desired Position
- Flip arrows, Move to Another View, Edit
Attachment, Align
Dimensions - Select the Dimension(s), then Right-Drag to
Desired
Function
- Add Text/Symbols, Tolerances, Change Text
Style, Etc - Select the Dimension-> Right-Drag to
Properties
- Trim Back Extension Lines - Select
the
Dimension,
and Drag Witness Lines to the Desired Position
- Add Notes - Insert Pulldown->Note
(or
)->No Leader/Leader->Make Note -> Follow the prompts
- Edit Notes - Select the Note->
Right-Drag->Properties
7) ADD SHEETS AND ADD/SET DRAWING
MODELS
- Add Sheets- Insert Pulldown->Sheet
- Remove Sheets- Edit
Pulldown->Remove
Sheet
- Reordering Sheets- Edit
Pulldown->Move
Sheet
- Move a View to Another Sheet- Select a
View->Edit
(Pulldown)->Move Item to Sheet->
- Add Drawing Model- Right-Drag on the
Sheet to Properties->Drawing
Models->Add Model->Select the Model
- Set Drawing Model- Right-Drag on the
Sheet to Properties->Drawing
Models->Set Model->Select the Model
8) UPDATE AND SAVE THE DRAWING
