Exporting and
Importing Solid Models with Pro/Engineer
STL File
Exports for Rapid Prototyping
It is often desirable to construct a physical
prototype of a project. Rapid Prototyping machines commonly require STL
formatted files as input. The STL files contain the part description as a
series of tetrahedral elements. (Do not mix-up the STL elements with FEM
elements, there is no connection between them).
File
– Save a Copy… and select as Type STL – OK
In the Export
STL window
select Binary,
for coordinate system select
Default.
Rapid prototyping machines
sometimes require only positive coordinates for the part description. One needs
to create a special offset coordinate system to accommodate those systems.
For a better resolution of
your model, decrease the default Chord Height before exporting and click Apply to see the effect. When
satisfied click OK.
NOTE:
The selection of the proper
chord height size is important for the faithful representation of the
underlying geometry of the part being built. As an example: A cord length of < 0.005 may be required to
reproduce some of our more intricate parts properly.
STL-exported part
Importing Files from other
CAD Packages
Importing foreign file to Pro/E is with Insert – Shared
Data – Data from File… and the
selecting the appropriate file.
The standard method to transfer solid models between
CAD packages is by the STEP file format. While this will port actual solid
parts, only newer CAD packages support this format. We can import a SoildWorks
2000 STEP file. As an example we will use fetch_proe
shovel.stp
to obtain a copy of such a file.
A more common method utilizes the IGES file format. Practically
all CAD packages support this file format. Note however, that this process
transfers surfaces only. In order to have Pro/E treat the model as a solid, one
has to convert the surfaces into a Protrusion.
Before one can convert the surfaces into a solid it might be necessary to fix
some boundaries or edges.
To look at this process we will take the IGES file
for a quarter-section a flywheel, created in Bentley's MicroStation, and import
it into Pro/E. (use fetch_proe wheel.igs to obtain a copy of this
file).
|
Imported Part |
Importing
an IGES File In Pro/E we create a new part with File - New name the part fwheel. Next use Insert – Shared Data – Data from File… and select file wheel.igs – click Close on Info window popping up. Next click on the Arrow icon in little window and select PRT_CSYS_DEF and click OK. Reorient the view to get a better front view of the model and change the display mode to wire-frame. At this stage you have imported the surfaces defining the wheel. All properly imported surfaces will appear in purple. If you find some line segments highlighted in pink, then this means you have unconnected edges. These need to be fixed before a successful conversion to a solid can be attempted. |
Our
model has this difficulty. To fix this quilt select the Import feature in the Model Tree and right-click it; from the
pop-up menu select Edit Definition. Notice a new entry in the top pull-down menu – Geometry.
Select from it:
Import
Data Doctor…
Now you will find some new
icons on right side of the top tool bar; select from it the Repair
Mode icon;
now you will find on the right side bar the Repair tool icon – click it. The dashboard is displayed
and you will see in the graphics window the repaired surfaces. Click Check in the dashboard and Check on the right to leave the Repair mode. The repair is complete click Check once more on the right to exit the Data
Doctor.
Notice the pink segments have
changed to purple now, the quilt is fixed. Now we can convert the quilt to a
solid. With the Import feature
selected in the Model Tree do:
Edit – Solidify… and then
Check
from the dashboard.
The successful conversion
will result in the model being displayed in white, the default color for a
solid. The model import is complete and ready for further work.
We might want to build a
complete model by mirroring the imported feature:
Select the part in the Model
Tree. The very first entry there and notice on the vertical right tool bar the
Mirror tool became active. Click on it:
Mirror -
select a surface to mirror; horizontal cut and
then Check
from the dashboard
resulting in the right half of the wheel.
Repeat this process once more and select the vertical
cut face; this will result in the complete wheel. Save it.