Tài liệu 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 Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 1 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. Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 2 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 Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 3 Intellectual Technology Limited Siemens NX 6 Surface Modeling - Mouse Let’s Start! Tutorial 2A • Create a new project folder (e.g. C:\projects\mouse) and copy the drawing file (mouse_outline_b.dxf) into the folder • Enter Siemens NX 6 by double-clicking its icon on the desktop • Select “Roles Essential with full Menus”, then click ok • • • File/New Select Model as Type Enter “master_model_a.prt” as file name Select the path of the project folder Click ok • • Version 1a – Feb 2010 Provide Expertise to Siemens NX Users in China and Hong Kong WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 4 Intellectual Technology Limited Siemens NX 6 Surface Modeling - Mouse Provide Expertise to Siemens NX Users in China and Hong Kong Tutorial 2A • • • 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) Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 5 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” Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Handle (free to move) Page 6 Intellectual Technology Limited Siemens NX 6 Surface Modeling - Mouse Provide Expertise to Siemens NX Users in China and Hong Kong Tutorial 2A • • • • • • • 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 • • • Select all curves of Right View Select “Move Handles Only” Draft the handle to the endpoint of the line • • • • • 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 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 7 Intellectual Technology Limited 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 Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited unTick Page 8 Intellectual Technology Limited Siemens NX 6 Surface Modeling - Mouse Provide Expertise to Siemens NX Users in China and Hong Kong Tutorial 2A • • • • Insert Datum/Datum plane Select xy plane Distance 50mm Click ok • • • • • • 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” • • • Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Mirrored point Draw a point here Page 9 Intellectual Technology Limited Siemens NX 6 Surface Modeling - Mouse Provide Expertise to Siemens NX Users in China and Hong Kong Tutorial 2A • • • • • Insert Datum/Datum plane Select xz plane Reverse Direction Distance 50mm Click ok • • • • • • 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” • • • Version 1a – Feb 2010 drag drag WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 10 Intellectual Technology Limited 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 • • 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) Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 11 Intellectual Technology Limited Siemens NX 6 Surface Modeling - Mouse Provide Expertise to Siemens NX Users in China and Hong Kong Tutorial 2A • • • • • • • • • • • • • • 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” Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 12 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 Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 13 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 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 • • • • Mirror a surface:Insert/Associative Copy/Mirror Body Select this surface as body Select yz plane as mirror plane Click ok result Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 14 Intellectual Technology Limited Siemens NX 6 Surface Modeling - Mouse Provide Expertise to Siemens NX Users in China and Hong Kong Tutorial 2A • • • • • • • • 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 Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 15 Intellectual Technology Limited Siemens NX 6 Surface Modeling - Mouse Provide Expertise to Siemens NX Users in China and Hong Kong Tutorial 2A • Hide Datum.3 • • • 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” • • • • • Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 16 Intellectual Technology Limited 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 • • • • 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” Version 1a – Feb 2010 Horizontal line(reference) Offset curve WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Coincided with y axis Page 17 Intellectual Technology Limited Siemens NX 6 Surface Modeling - Mouse Provide Expertise to Siemens NX Users in China and Hong Kong Tutorial 2A • • • • • Insert/Datum/Datum plane Select XZ plane Select the endpoint Select “Associative” Click ok • • • • • 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” • • • Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 18 Intellectual Technology Limited Siemens NX 6 Surface Modeling - Mouse 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 • • • • • • 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 Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 19 Intellectual Technology Limited Siemens NX 6 Surface Modeling - Mouse Provide Expertise to Siemens NX Users in China and Hong Kong Tutorial 2A • • • • • • • 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 • • • Specify four points as variable radius points Enter values as shown Click ok 3mm 7mm 3mm Version 1a – Feb 2010 WWW.ADVANCECAD.edu.vn Copyright © 2010 by Intellectual Technology Limited Page 20