Friday, September 15, 2017

Siemens Nx Tutorial--Unified National Fine (UNF) Thread profile (Along with audio narration)

Siemens Nx Tutorial--Unified National Fine (UNF) Thread profile

Hello viewers in this tutorial, we are going to create a Unified National Fine (UNF) Thread profile in Siemens Nx software. External and Internal profiles will be created separately. That would be used in creating Bolt and Nut which will be demonstrated later in another video.

 

Video Transcription

  1. Start a new file using inch units.
  2. Fill the name of the file UNF Screw External Thread Profile.
  3. Create a new sketch over XZ plane.
  4. Before starting the sketch we will set some preferences of the software.
  5. Here in Drafting Preference under the text, set the decimal places of units to 5 and ‘Decimal Delimiter’ to the period instead of a comma.
  6. Create a line and apply a dimension of 1/20 inches to it.
  7. Apply a coincident constraint between the midpoint of this line and sketch origin.
  8. Switch to Tools Tab and click over the ‘Expression’ command, here you can see the last dimension we applied over the line, named p0, change its name to Pitch which will be used as constant later.
  9. Convert this line to a reference line.
  10. Create two more lines in the sketch and apply a 60° angle between them.
  11. We can see a vertical constraint has been automatically applied by the software between the intersection of newly created two lines and sketch origin.
  12. Convert these two lines into reference line.
  13. Create two more lines parallel to the previous lines as shown here.
  14. Apply between horizontal constraints between the endpoints of these lines and convert them into reference lines.
  15. Create another reference line and apply a horizontal constraint over it.
  16. Apply a dimension of Pitch/6 over it.
  17. In the same way, create another reference line collinear to the previous line on the other side.
  18. Next add another reference line over here and apply a dimension of Pitch/8 over it.
  19. Activate Arc tool and draw an arc tangent to these three lines and apply constraints as required.
  20. Next, draw another arc coincident to the midpoint of this line and tangent to the adjacent line by applying constraints.
  21. Mirror this arc to the other side using Mirror Curve tool.
  22. Connect these arcs using lines to complete the sketch which we require.
  23. Here we can see an auto dimension is still applied which means something is missing.
  24. Fully constrain the sketch by applying a horizontal constraint over this line.
  25. The sketch is complete so exit the sketch and save it.
  26. Addition to this we need to create another Thread Profile for the Internal screw too, to do so, save as, this file with the name ‘UNF Screw Internal Thread’ Profile.
  27. So we can see the file saved as for Internal Thread Profile is currently active next make some changes in the sketches.
  28. Delete these sketches.
  29. Change the value of this dimension to Pich/4.
  30. Draw these lines using Profile Tool as shown.
  31. Here apply a coincident constraint between the endpoints of the line which was not created automatically.
  32. See the sketch is now fully constrained.
  33. Chang back this reference line into normal line.
  34. Our sketch is complete so exit from the sketching mode.
  35. Save the file.

download-Link

 

Visit the following link to get the model file…
http://autode.sk/2jt0hi8

 


....................................................................................

Visit the following link to watch more tutorial on Siemens NX by us

https://www.youtube.com/playlist?list=PLKWX3xUP3pPpUvtPuzEPoHimjTjpdbl_Q

.........................................................................

Hope all of you enjoyed the tutorial. If you find the video useful please like it and share it with your friends/colleagues and do not forget to subscribe me to get latest updates about my new uploads….

http://www.youtube.com/user/nisheethsorjm?sub_confirmation=1

Wednesday, September 6, 2017

Engine MKII (Volume-1) Siemens NX Tutorial

Engine MKII_1

Engine MKII_2

Serial No. 100-A.

Engine MKII (Volume-1) Siemens NX Tutorial

The Design of this model has been taken from Assembly file of 'Rear Exhaust-2 Shoe' of ‘Sample files’ of Autodesk Inventor, it is a fragment of ‘Engine MKII’ Assembly.
(Rest of the Assembly is designed in Volume-2)
.................................................................................................
Rest components of the model ‘Engine MKII Assembly’ (consisting of several numbers) have also been designed. You may watch them by visiting on the following playlist:-
https://www.youtube.com/playlist?list=PLKWX3xUP3pPplOPikb5S8WD4re7tAnT3-
.................................................................................
In this Siemens NX11 Assembly tutorial, we have created a model named ‘Engine MKII’. The Assembly consist of 2 Subassemblies and 38 parts that are positioned according to design intent by using Assembly Constraints. Tutorial watch how an assembly of engine components is created by using different mates.
The animation of internal components is also accomplished after setting all the components.
To complete this tutorial, first get the files used for creating the assembly.
This tutorial will give you a good practice of applying constraints in an assembly and give you an idea of Engine MKII mechanism.
The video covers following assembly modelling techniques:--
_____________________________________________________________
• Use the Assembly commands such as Add Components, Assembly Constraints, and Move Component with Triad tools etc.
• 38 Parts will be inserted with the help of ‘Add Component’ tool.
• Use the Touch/Align, Fix, Align/Lock and Angle constraints between the two components etc.
• How to create two different views of assembly components, one will be visible only internal components and other visible all components by using the ‘Arrangements’ command.
• Animate the internal components like an Engine Piston, Crank shaft, Connecting rod of Engine with the help of ‘Insert Motion’ command in the Assembly Sequence task environment.

download-Link

 

 

Click the following link to get the model file: - http://autode.sk/2iXSjxd