Siemens Nx Tutorial || Bolt and Nut with creation of thread manually|| Along with audio narration
Hello viewers in this tutorial, we are going to create a bolt and nut of ½ inch dia where we will create threads manually using a Unified National Fine (UNF) Thread profile of 1/20 inch pitch. We will create using equations so that by changing the dia, length and pitch the size of bolt and nut can be modified. To show how it can be done we will also create a bolt of 3/8 inch dia having a pitch of 1/24 inches by changing the parameters using the expression command. In a previous tutorial, we demonstrated how to create UNF Thread Profile. Video Transcription Start a new model file using inch units. Fill the name of the file Bolt. Switch to ‘Tools Tab’ and activate ‘Expressions’ command. Create a new expression named D and fill ½ inches in Formula, click ok to exit from the command. Start a new sketch over YZ plane. First set some preferences of the software. Here in Drafting Preference in the Text Units under Dimension settings, set the decimal places of units to 5 and ‘Decimal Delimiter’ to the period instead of a comma. Draw a polygon and apply a vertical constraint on its this side. Apply a dimension of D*1.5 over here on this polygon and exit from the sketching mode. Extrude this sketch profile and in ‘End Distance’ field fill value D*0.634. Change the colour of the model using ‘Edit Object Display command available at ‘View Tab’. Edit the colour of the model and apply a custom colour by filling the values 247 in Red, 225 in Green and 182 in Blue input dialogue box. Create a new sketch over XZ plane of the model and draw a sketch using ‘Line Tool’ as displayed. Apply a dimension of D*1/8 over this line and an angle of 30° between both lines. The sketch is complete so revolve it and remove the material from the solid. Create a sketch, over this face of the model and activate Static Wireframe view mode. Draw a circle coincident to the origin of the model. Apply a tangent constraint between the circle and this edge of the model. Re-activate ‘Shaded with Edges’ view mode. Create another circle in the sketch and apply an offset dimension of D*1/16 between these circles. Convert this circle into reference geometry and exit from the sketching mode. Extrude this sketch and in Extrude dialogue box fill the ‘End Distance’ 1/64 and in offset option select Two-Sided. In offset distance at end value box, fill 0.25 inches and execute the command after reversing the direction of Extrude. Create a new sketch over following face of the model and draw a circle coincident with the sketch origin next apply a dimension D here. Exit from the sketching mode and Extrude this sketch up to 2 inches. Hide the visible of sketches and save the file. Apply a chamfer over the following edge of the model, having 1/32 inches of length and 45 degrees of angle. Create a new sketch over XZ plane. Activate Intersection Curve command and select following face of the model. Here you can see in selection filter Curve option is selected which means while making a selection only sketch curves will be selected. Select all the curve present in the sketch and convert them into reference geometry. Draw two reference lines in the sketch as displayed and exit from the sketching mode. Next, open the folder named UNF Screw Thread Profiles from your hard drive. Check the video description and Youtube Cards to find the files required to complete this tutorial. From here open file named ‘UNF Screw External Thread Profile’. Here edit sketch which is visible in front of you. Select these arcs and lines. Activate copy command from the right-click menu to copy the selected sketches to the clipboard. Exit from the sketch and switch back to Bolt file. Edit the last sketch we created and paste the sketch which is present in the windows clipboard. Activate ‘Profile Tool’ and add these lines to the profile so that it clearly intersect the solid created up till now in the file. Select the thread profile sketch after activating sketch filter as a curve. Activate Move Curve tool. First, verify that ‘Angle’ is selected in ‘Transform Motion’ type. Next, specify Axis Point as displayed. Then fill 180° and click apply. Now in Transform Motion type select Point to Point. First, specify ‘from’ point and then specify ‘to’ point as displayed. Select sketches to be moved and click ok. Exit from the sketching mode. Switch to Analysis Tab and activate Measure Distance Command. Measure the total length of the bolt as displayed, that is 2.3170 inch. Activate Helix Cure Tool from Curve Tab. In the X, Y, Z coordinate position of the curve, fill the last measured distance 2.3170 inches in X input field and rotate the curve by -90°. The diameter of the curve should be 0.5 inches, in pitch fill the value 1/20+0.001 and length of the curve should be 1.25 inches. In the start angle, fill a value so that start point of curve coincident with the UNF thread profile. Activate Swept Tool and first select the thread profile, next Helix curve as guides. Verify that ‘Orientation Method’ is selected as ‘Vector Direction’ and then define vector direction as displayed. Click Ok to execute the command. Hide the visibility of sketches and curves. Activate Subtract Tool, select bolt as target body and swept feature as a tool body. Execute the command and threads are created in front of us. Hide everything in the file except solid bodies. The file is complete so save it. Let us see how we can change the size of the bolt by changing some parameters using references command. We will change the dia of the bolt to 3/8 inches and pitch of threads to 1/24 inches. First, suppress Swept and Subtract feature because these features will not update automatically after changing the parameters. Activate Expressions
Siemens Nx Tutorial–Unified National Fine (UNF) Thread profile (Along with audio narration)
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 Start a new file using inch units. Fill the name of the file UNF Screw External Thread Profile. Create a new sketch over XZ plane. Before starting the sketch we will set some preferences of the software. 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. Create a line and apply a dimension of 1/20 inches to it. Apply a coincident constraint between the midpoint of this line and sketch origin. 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. Convert this line to a reference line. Create two more lines in the sketch and apply a 60° angle between them. We can see a vertical constraint has been automatically applied by the software between the intersection of newly created two lines and sketch origin. Convert these two lines into reference line. Create two more lines parallel to the previous lines as shown here. Apply between horizontal constraints between the endpoints of these lines and convert them into reference lines. Create another reference line and apply a horizontal constraint over it. Apply a dimension of Pitch/6 over it. In the same way, create another reference line collinear to the previous line on the other side. Next add another reference line over here and apply a dimension of Pitch/8 over it. Activate Arc tool and draw an arc tangent to these three lines and apply constraints as required. Next, draw another arc coincident to the midpoint of this line and tangent to the adjacent line by applying constraints. Mirror this arc to the other side using Mirror Curve tool. Connect these arcs using lines to complete the sketch which we require. Here we can see an auto dimension is still applied which means something is missing. Fully constrain the sketch by applying a horizontal constraint over this line. The sketch is complete so exit the sketch and save it. 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. So we can see the file saved as for Internal Thread Profile is currently active next make some changes in the sketches. Delete these sketches. Change the value of this dimension to Pich/4. Draw these lines using Profile Tool as shown. Here apply a coincident constraint between the endpoints of the line which was not created automatically. See the sketch is now fully constrained. Chang back this reference line into normal line. Our sketch is complete so exit from the sketching mode. Save the file. 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
Engine MKII (Volume-1) Siemens NX 11 Tutorial
Serial No. 100-A. Engine MKII (Volume-1) Siemens NX 11 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. Click the following link to get the model file: – http://bit.ly/30VamVp
Engine MKII (Volume-2) Siemens NX 11 Tutorial
Serial No. 100-B. Engine MKII (Volume-2) Siemens NX 11 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.(Starting of the Assembly is designed in Volume-1)…………………………………………………………………………………….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. Click the following link to get the model file: – http://bit.ly/30VamVp
Engine MKII (Volume-2) Solid Edge ST9 Tutorial
Serial No. 104-B. Engine MKII (Volume-2) Solid Edge ST9 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.(Starting of the Assembly is designed in Volume-1) 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=PLKWX3xUP3pPrb1bU6P_goEUCMvcfTuqtI………………………………………………………………………In this Solid Edge ST9 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 mechanism.The video covers following assembly modelling techniques:–_____________________________________________________________• Use the Assembly commands such as Insert Components, Mate, and Drag Component with Triad tools etc.• 38 Parts will be inserted with the help of ‘Insert Component’ tool.• Use the Mate, Planer Align, Connect and Angle constraints between the two components etc.• Check the interference between the two components by using ‘Check Interference’ tool.• Save different state views of an assembly the internal components of engine easily by using the ‘Alternate Assemblies command.• Animate the internal components like an Engine Piston, Crank shaft, Connecting rod of Engine with the help of Rotational Motor command in the Simulate Motor environment. Click the following link to get the model file: – http://bit.ly/2MtNAi6
Engine MKII (Volume-1) Solid Edge ST9 Tutorial
Serial No. 104-A. Engine MKII (Volume-1) Solid Edge ST9 Tutorial Engine MKII (Volume-1) Solid Edge 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=PLKWX3xUP3pPrb1bU6P_goEUCMvcfTuqtI………………………………………………………………………In this Solid Edge ST9 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 mechanism.The video covers following assembly modelling techniques:–_____________________________________________________________• Use the Assembly commands such as Insert Components, Mate, and Drag Component with Triad tools etc.• 38 Parts will be inserted with the help of ‘Insert Component’ tool.• Use the Mate, Planer Align, Connect and Angle constraints between the two components etc.• Check the interference between the two components by using ‘Check Interference’ tool.• Save different state views of an assembly the internal components of engine easily by using the ‘Alternate Assemblies command.• Animate the internal components like a piston, crank shaft, connecting rod of Engine with the help of Rotational Motor command in the Simulate Motor environment. Click the following link to get the model file: – http://bit.ly/2MtNAi6
Miscellaneous Components of ‘Engine MKII’ (Siemens NX 11 Tutorial)
Serial No. 99 Miscellaneous Components of ‘Engine MKII’ (Siemens NX 11 Tutorial) The Design of these components ‘Engine Wrist Pin’, ‘Rear Exhaust Manifold Seal’ and ‘Coupling Rear’, have been taken from Assembly file of ‘Rear Exhaust-2 Shoe’ of ‘Sample files’ of Autodesk Inventor, it is a fragment of ‘Engine MKII’ Assembly.Parameters are used to create the Extension Spring through Expressions command.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-……………………………………………………………………………Inside this video, you can see the full detailed process of making 3-D Parametric CAD Model through Siemens NX 11. Click the following link to get the model file: – http://bit.ly/2pUnA86
Miscellaneous Components of ‘Engine MKII’ (Solid Edge ST9 Tutorial)
Serial No. 103 Miscellaneous Components of ‘Engine MKII’ (Solid Edge ST9 Tutorial) The Design of these components ‘Engine Wrist Pin’, ‘Rear Exhaust Manifold Seal’ and ‘Coupling Rear’, have 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 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=PLKWX3xUP3pPrb1bU6P_goEUCMvcfTuqtI……………………………………………………………………………Inside this video, you can see the full detailed process of making 3-D Parametric CAD Model through Solid Edge ST9. Click the following link to get the model file: – http://bit.ly/2pa0r0N
Extension Spring 3.873 (Siemens NX 11 Tutorial)
Serial No. 98 Extension Spring 3.873 (Siemens NX 11 Tutorial) The Design of the model ‘Extension Spring 3.873’ 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.Parameters are used to create the Extension Spring through Expressions command.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-……………………………………………………………………………Inside this video, you can see the full detailed process of making 3-D Parametric CAD Model through Siemens NX 11. Click the following link to get the model file: – http://bit.ly/2AQmdJJ
Extension Spring 3.873 (Solid Edge ST9 Tutorial)
Serial No. 102 Extension Spring 3.873 (Solid Edge ST9 Tutorial) The Design of the model ‘Extension Spring 3.873′ 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. Parameters are used to create the Extension Spring through Variables command.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=PLKWX3xUP3pPrb1bU6P_goEUCMvcfTuqtI……………………………………………………………………………Inside this video, you can see the full detailed process of making 3-D Parametric CAD Model through Solid Edge ST9. Click the following link to get the model file: – http://bit.ly/33mPFDz
