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
