Mô tả:
Free-Siemens-NX-(Unigraphics)-Tutorial---Surface-Modeling
Intellectual Technology Limited
Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Siemens NX 6 Surface-modeling
(Tutorial 2 – Mouse)
Surface-modeling
Solid-modeling
Assembly Design
Design with a Master Model
Design in Context
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Intellectual Technology Limited
Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
- Import 2D outline drawing into Siemens NX 6
- Build 3D curves based on the imported drawing
- Build the upper surfaces of the mouse
Tutorial 2B
- Do the draft analysis to search any undercut portion on the upper surfaces
- Build the lower surfaces of the mouse
- Convert the surfaces into a solid (Master Model)
Tutorial 2C
- Build the parting surfaces based on the imported drawing
- Create components from the finished model
- Create a new part in the assembly (Design in Context)
- Modify a part design while looking at other parts (Design in Context)
Please be reminded that this series of tutorials is designed to demonstrate a design approach with
Siemens NX, rather than the command itself. For the details of commands, please read the online
help or attend the software training.
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Intellectual Technology Limited
Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Intellectual Technology Ltd is a regional value added reseller of Siemens PLM solutions. We enable our customers with innovative
and collaborative design, engineering, manufacturing, simulation tools.
What ITL can do for you:
1. Engineering Design & Development
a. Conversion of 2D data into 3D model
b. Detailing and Drafting of products for manufacturing with tolerances and surface finishes, Assembly layout drawings
and BOM creation
c. Reverse Engineering - Creation of accurate product models and detailed drawings using CMM and scanning techniques
2. NX Solution Training
a. NX Basic & Advanced Design trainings
b. NX CAM Programmer Training
c. NX Mould Design/Electrode Design
d. Other Customized training
3. NX CAM Post Processor Development
We provide services of post processor customization and development for the following machines
a. 3 Axis , 4 Axis and 5 Axis Milling
b. Turning, EDM and Wire EDM
4. NX Solution Maintenance and Support
We provide NX solution annual maintenance and support to our customers. This solution maintenance includes the
following major services:
a. Dedicated Application Engineer to Support the solution.
b. On-site solution support
c. Solution upgrades, upgrade trainings
d. Free phone enquiries
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Intellectual Technology Limited
Siemens NX 6 Surface Modeling - Mouse
Let’s Start!
Tutorial 2A
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Create a new project folder (e.g.
C:\projects\mouse) and copy the
drawing file (mouse_outline_b.dxf) into
the folder
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Enter Siemens NX 6 by double-clicking
its icon on the desktop
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Select “Roles Essential with full Menus”,
then click ok
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File/New
Select Model as Type
Enter “master_model_a.prt” as file
name
Select the path of the project folder
Click ok
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Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
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Double-click on the default Datum
coordinates system
Select “Absolute CSYS” as type
Click ok
Double-click to edit
To Import the outline drawing:• File/Import/DXF
• Select the file “mouse_outline_b.dxf”
• Select “WORK” as “Import to Part”
• Click ok
(the imported curves will be pasted on the
XY plane)
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Intellectual Technology Limited
Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
To confirm that the size of the drawing is correct:• Double-click on the scale line of the drawing
• Check if the displayed length is 50mm; if not, we
need to enlarge or shrink the drawing into the
correct size
• Delete the scale line ( we don’t need it anymore)
To Reposition the 3 views (offset from absolute
datum by 150mm):• Edit/Move Objects…
• Select all the curves of Top View
• Select “Move Handle Only”
• Drag the handle to the midpoint of the arc
• Deselect “move handle only”
• Select “Move Original”
• Enter x =0. y=0, z=150
• then rotate about z by 90deg (clockwise)
• Click “Apply”
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Handle
(free to move)
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Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
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Select all curves of Front View
Select “Move Handles Only”
Draft the handle to the midpoint of the line
Deselect “move handles only”
Enter x =0, y= -150, z=0
Then rotate about x by 90deg (as shown )
Click apply
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Select all curves of Right View
Select “Move Handles Only”
Draft the handle to the endpoint of the line
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Deselect “move handles only”
Enter x =150, y= 2.85, z=0
Then rotate about x by 90deg (as shown
Rotate about z by 90deg (as shown )
Click ok to complete
Version 1a – Feb 2010
Top
View
Right
View
Front
View
)
Result
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Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
To Change all curve colors to Yellow:• Select all curves
• Right-click on a curve, select “edit display”
• Select “Yellow” as Color
• Click ok
To Move all curves to a layer99:• Select all curves
• Select “Format/ Move to Layer…”
• Enter 99
• Click ok
To make all layers Invisible, except layer 1, 61&99:• Format/Layer Settings…
• UnTick all layers, except 1, 61, & 99
• Select “visible only” for layer99
• Click close
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unTick
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Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
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Insert Datum/Datum plane
Select xy plane
Distance 50mm
Click ok
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Insert/Sketch…
Select the offset plane
Click ok
Draw a point as shown
Mirror the point around y axis
Draw a 3-point arc (start & end at the
existing points, middle at the origin)
Drag the endpoint to make it longer
(the arc should match the reference)
Click icon “Finish Sketch”
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Mirrored point
Draw a point here
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Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
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Insert Datum/Datum plane
Select xz plane
Reverse Direction
Distance 50mm
Click ok
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Insert/Sketch…
Select the offset plane
Click ok
Draw a point as shown
Mirror the point around z axis
Draw a 3-point arc (start & end at the
existing points, middle on the yellow arc)
Drag on the curve to adjust radius
Drag an endpoint to make it longer
Click icon “Finish Sketch”
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drag
drag
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Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
To build a 3d curve by combined projection :• Insert/ Curve from Curves/ Combined
Projection
• Select sketch.0 as curve.1
• Select sketch.1 as curve.2
• (projection direction = normal to curve)
• Click ok
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Sketch.0
Sketch.1
Hide Sketch.0 & Sketch.1 (right-click, select
“hide”)
Hide Plane1 & Plane2
(This combined curve can fit the shapes of both
top view and front view)
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Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
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Insert/Datum/Datum plane
Select yz plane
Switch to Top View
Drag the plane onto the plane (we can drag
the green ball to make the plane bigger)
(offset value = 30.5)
Click ok
drag
Insert/Sketch
Select the offset plane, click ok
Draw two arcs (tangent to each other)
Click icon “Constraints”
Select the end point and the absolute y axis
Select “point on curve” (the endpoint is now
on y-axis)
Adjust the shape & position of the arcs so that
they can match the yellow reference
Click icon “finish sketch”
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Intellectual Technology Limited
Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
To Create an extruded surface:• Insert/Design Feature/Extrude…
• Select the combined curve as Section
• Select +Z as the direction
• Enter 20 mm as distance
• Click ok
To Create a Draft 5 deg (from parting line):• Insert/Detail Feature/Draft
• Select “From Edges” as type
• Select +Z as Draw Direction
• Select the lower edge
• Enter 5 deg as Angle 1
• Click ok
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Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
To Create an extruded surface with Draft:• Insert/Design Feature/Extrude
• Select “Sketch.2” as Section
• Select +Z as the direction
• Enter 20 mm as distance
• Select “From Start Limit” as Draft
• Enter 5 deg as Angle
• Click ok
To
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Mirror a surface:Insert/Associative Copy/Mirror Body
Select this surface as body
Select yz plane as mirror plane
Click ok
result
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Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
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Insert/Detailed Feature/Face Blend
Select surface as Chain1
Select surface as Chain2
(Both arrows should point inward; if not,
reverse it)
Enter 5mm as Radius
Select “Trim to all input faces”
Click ok
Repeat the above steps for the opposite
side
result
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Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
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Hide Datum.3
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Insert/Sketch
Select XZ plane, click ok
Insert/ Curve from Curves/Offset from
curve
Select the combined curve
3.5 mm as offset value
Click ok
(We can create an offset curve from any
entity that is out of the sketch.)
Click icon “Finish Sketch”
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Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
To create a sketch mating with an external sketch:• Insert/Sketch
• Select yz plane
• Draw two arcs as shown (tangent to each
other)
• Draw a horizontal line starting from the
connecting point , then make either one
tangent to it; Convert the line to a reference
line
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Create an intersection point
on the offset
curve (Insert/Curve-from-curves/intersection
point)
Make a “Point on curve” constraint
Adjust the shape & position of the arcs so that
they can match the yellow reference (just drag
on curves or points)
Click icon “finish sketch”
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Horizontal
line(reference)
Offset curve
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Coincided
with y axis
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Siemens NX 6 Surface Modeling - Mouse
Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
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Insert/Datum/Datum plane
Select XZ plane
Select the endpoint
Select “Associative”
Click ok
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Insert/Sketch
Select the offset plane, click ok
Draw a point as shown
Mirror the point around Z axis
Draw a 3-point arc (start & end at the two
points, middle at the point
)
Drag on the curve to adjust radius
Drag the endpoint to make it longer
Click icon “Finish Sketch”
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Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
To Create a Swept surface ( 1section & 2
guides):• Insert/Sweep/Swept
• Select “Single Curve” on selection filter
• Select Curve as Section
• Select Curve as Guide 1
• Click “Add new set”
• Select Curve as Guide 2
• Click ok
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Insert/Trim/Trim-and-Extend
Select “Make Corner” as type
Select a surface as Target
Select the other surface as Tool
Reverse arrows so that the result is as
shown
Click ok
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Provide Expertise to Siemens NX Users in China and Hong Kong
Tutorial 2A
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Insert/Trim/Trim body
Select the surface as Target
Select Plane as Tool
(arrow should point backward; if not,
reverse it)
Click ok
Insert/Detail-Feature/Edge Blend
Select an edge (all tangent edges are
selected automatically; selection filter =
tangent curves)
7mm
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Specify four points as variable radius points
Enter values as shown
Click ok
3mm
7mm
3mm
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