Animation displayed in Ceiling Hook — SolidWorks 2014 (with caption and audio narration)
Serial No. 214 Animation displayed in Ceiling Hook — SolidWorks 2014 (with caption and audio narration) In this video, we will demonstrate how to apply the different type of mates in the assembly environment for creating the animation. ……………………………………………………………………….To watch full sketching video of this model ‘Ceiling Hook’, please visit on my another associated video named as ‘Ceiling Hook with Animation’ (SolidWorks). Click the following link to get the model file: – http://bit.ly/31K8Bvu Transcription of the Video Create a new assembly file. The ‘Begin Assembly’ command is already activated in the assembly design window. Click Browse button, place the part file ‘Hook’. First of all, open the visibility of ‘View Origin’ of the assembly. Click the View Origin point button to place the file, centre of the assembly. Choose ‘Isometric View’. In the same way, place one more part file-name ‘Circular Ring.’ Rotate the part by using ‘Move with Triad’ tool. Save the assembly with the name ‘Ceiling Hook’ and edit the ‘Hook’ part file. Create a new sketch over the ‘Front Plane’ and take a project of this circular edge by using ‘Convert Entities’ command. Finish the sketch and return back to the assembly environment. Select the Front Plane of assembly and Right Plane of Circular Ring and mate it. It will apply a Coincident mate. Move the Circular Ring slightly. Activate the ‘Mate’command, select tangent face of Circular Ring and arc along the path of hook, and apply the tangent mate. Select the Front Plane of Circular Ring, Right Plane of assembly and apply the Coincident mate. Edit the Circular Ring part and activate the Axis tool. Choose ‘Point and Face/Plane’ option as this particular type of selection. Many options available here, choose any option as you need. Select the origin point and Front Plane of assembly to create the axis. Click OK to execute the command. Open the visibility of axis by using ‘View Axes’ command. Return to the assembly view. Activate the ‘Mate’ command, select the assembly origin and Axis of Circular Ring and apply it. Select the Coincident2 mate and suppress the mate. Let see here, the Circular ring part rotates about the inner periphery of Hook with the help of tangent and axis mate. Create an Axis between origin point of assembly and end point of arc in assembly. Create a new work plane between front plane and this axis. A work plane has been created along the axis. Apply an angle mate between Front plane of Circular Ring and Plane1. Set the angle value to 0 degree. Go on the Evaluate tab and activate the ‘Measure’ command. Select the Top Plane and Plane1 and monitor the value. Copy the angle value and calculate the value as shown (290.39126 degree). In the next section, we will create animation on the Circular Ring its start value is 00 and end value 290.391260. Choose Front View, in the Orientation dialog box, activate the ‘New view’ command and set its name as ‘View2′. In the same manner, choose Isometric View, set its name as ‘View1’. These saved views will be used later in animation timeline. Select the Motion Study tab, click the Orientation and Camera button in the animation timeline. Right click on the time bar and select Move Time Bar option, set the time on 2 second. Copy the View-1 key and place the key on 2 seconds. Pause 2 seconds on the View-1 position. Move the time bar on 7 seconds and add the new key. Minimize the animation timeline and choose View-2, in the Orientation dialog box. Return back to the animation timeline and right click over the 7 seconds key and select ‘Replace Key’ option. Time taken 5 seconds in changing from view-1 to view-2 position. In the Mates folder, select the Angle1 mate and add the key in the timeline by using Add key button. Right click the animation timeline, move the time bar at 22 seconds. Right click on the Angle1 and select Edit Dimension option, paste the specified angle, click OK. Click the ‘Collapse Motion Manager’ button. Click play animation button to check the motion. Now we will create some modifications in the animation. Right click the start key point time of angle mate and move the key position at 9 seconds in the Edit time dialogue box. Right click the end key point time of angle mate and move the key position at 24 seconds. Stop the animation 2 seconds between View-2 and starting key point of Angle1 mate. Go on the Orientation and Camera tab, copy the View-2 key and paste the key over 24 seconds in the timeline. Move the time bar at 26 seconds, right click and paste View-2 key. Pause the animation for 2 seconds at View-1 position. Copy the end key point of Angle1 mate and paste key on 26 seconds. Stay in the still position for 2 seconds. Repeat the whole animation in reverse order to come back in starting position. Minimize the animation timeline and clear the screen. Click ‘Play from Start’ button and start the animation. Return back to the assembly environment and save the file.
iTwist Drill — Autodesk Inventor 2013 Tutorial (with caption and audio narration)
Serial No. 288 iTwist Drill — Autodesk Inventor 2013 Tutorial (with caption and audio narration) In this part modelling tutorial of ‘Autodesk Inventor,’ we will create a model named ‘iTwist Drill ’. We will start our work by defining some User Parameters that will be used to create a mathematical relation between the dimensions applied in the due course of modelling the ‘Twist Drill’. Then we will create a circle and extrude it. Next, we will create some user-defined work planes at specified spots. These planes will be used to draw some more sketches, to be used as a base profile for cutting flute (rounded grove) over the round bar. Then a coil feature and an extrude feature with a cut operation will be applied to create flute. Then using a circular pattern tool we will duplicate the same at an angle of 180°. Next, we will create some sketch profiles to cut lip and lip relief on the edge of the drill bit. The process will be the same as applied earlier. Later more coil feature will be applied to complete the model. The highlight of the videos is the after creating the model with full parameters the iPart creation of the model is also displayed. Watch the video to understand all the process clearly ……………………………………………………….. To more understand the creation process of an iParts in Autodesk Inventor watch a related video at the following link:— https://youtu.be/KNCrDJdPm-s. Click the following link to get the model file: – http://bit.ly/2mFTa8o Transcription of the Video Create a new inch part file. Go to the Manage tab and activate the ‘Parameters’ command. Add the Parameter name ‘diaMajor’ in the ‘User Parameters’ tab by using ‘Add Numeric’ key and set the value 7/16 ul in the equation area. In the same manner, add two more parameters and click OK. Create a new sketch over XY Plane. Create a circle and place the dimension, select the ‘List Parameters’ and choose diaMajor and click OK. Right-click the dimension and select ‘Expression’. Finish the sketch and activate the ‘Extrude’ command. The sketch profile will automatically select and set the distance value relating in terms of parameters, click OK. Save the file as ‘iTwist Drill’. Change the colour of the model as you wish. Activate the ‘Plane’ command and create a plane inside from this face. And place the dimension. Change the name of the plane as ‘ShankEnd’ and create an Axis in the centre of the part, name it as majorAxis. Activate the Axis command and select WorkPlane1 and XZ plane. A new axis will form on the intersection of these two planes. Change the name of this axis, call it as ‘Intersection Helix Origin Planes’. Now activate the ‘Point’ command and create a work point at the intersection of this vertical plane and axis . Activate the ‘Parameters’ command and add HelixAngle in the ‘User Parameters’ tab with the help of ‘Add Numeric’ button. Now see, different kinds of measurement options are visible here, you choose only one option at a time as per your design. In the Unit Type dialogue box, select degree option and click OK. Set the Helix angle to 30 degrees and click OK. Activate the ‘Plane’ command and select ‘Intersection Helix Origin Planes’ axis and XZ Plane, set the specified angle relating to parameters. Change the name of this plane, as ‘helix Origin Plane1’. Close the visibility of ‘ShankEnd’ plane and ‘Intersection Helix Origin Planes’ axis. Add two more parameters name as ‘web’ and ‘diacutter’. Create a new sketch on this plane. Rotate the model parallel to the inclined plane by using ‘Look at Plane’ command. Activate the slice graphics command. Take the project of ‘Intersection Helix Origin Planes’ and ‘Work Point1’ with the help of ‘Project Geometry’ command. Create a circle and set the desired dimensions to fully constrain the sketch. Finish the sketch and change the name of the sketch as ‘diacutter’. Add one more parameter call it as ‘helixPitch’. Activate the ‘Coil’ tool, it will automatically select the sketch profile, select the major axis and select the ‘Cut’ option in the Coil dialogue box. Go to the Coil Size tab and select the ‘Pitch and Height’ option. In the Pitch area select from the List Parameters click ‘HelixPitch’ and in the Height area select from the List Parameters, click ‘fluteLen+diaMajor’. Click OK to create the coil feature. Open the visibility of ‘diacutter1’ sketch. Activate the ‘Extrude’ command, select the ‘All’ option in the Extents field and choose ‘Cut’ option and click OK. Change the name of this extruded cut feature as ‘blend’. Activate the ‘Circular Pattern’ tool and select the Coil1 and blend feature from the browser bar, select the major axis as a rotation axis and fill the value of Occurrence count and angle. Click OK to execute the command. Create a new sketch on this face. Take the project of these four curves and circle. Draw a circle and tangent it to this curve. Select all the sketches and convert it construction geometry. Create two points on the intersection point of this circle and curve. Draw a line passing through the centre of the circle and add coincident constraint between line and point. Take the project of ‘Intersection Helix Origin Planes’ axis. Set the angular dimension between these two lines. Finish the sketch and change the name of the sketch as ‘TipRef1’. Make a Work Axis on this line. Change the name of the axis as ‘lipReliefGeom’. Activate the ‘WorkPlane’ command and select these two axes. Change the name of the plane as ‘lipReliefGeom’. Now the plane is created along the axis. Activate the ‘Angle to Plane around Edge’ command. Select the ‘lipReliefGeom’ plane and ‘majorAxis’, set the angle 90 degrees, click OK. Add the parameter ‘tipangle’ and set the angle 118 degrees. Create a new sketch over the ‘lipReliefGeom’ plane. Activate slice graphics command, take the project of this edge and major axis. Draw a vertical line and add coincident constraint between
Square Bend Tube through Sheet Metal — SolidWorks 2014 Tutorial (with caption and audio narration)
Serial No. 15 Square Bend Tube through Sheet Metal — SolidWorks 2014 Tutorial (with caption and audio narration) Inside this video, viewers will watch the full detailed process of creating this model through SolidWorks Sheet Metal design functionality. Click the following link to get the model file: – http://bit.ly/2uvJjpt Transcription of the Video Create a new Part file. Go to the ‘Edit Document Units’ tab and select ‘MMGS’ option. Create a new sketch over the Front Plane. Create a centre rectangle coincident with the origin and affix the dimensions. Select a horizontal line and convert into construction geometry. Draw two horizontal lines and apply the dimensions. Finish the sketch and choose the Isometric view. Save the file with the name ‘Square Bend Tube’. Create a new sketch over the Right Plane. Select the Right Plane and choose ‘Normal To’ option to rotate the view along the plane. Create a horizontal line and Vertical line with the preferred dimension. Create another line and set the angular dimension. Select these two lines and apply the equal constraint. Convert the four lines into construction geometry. Create two arcs between the endpoint of lines. Finish the sketch and activate the ‘Swept Flange’ command. In the Profile selection area, select the rectangle in the graphics area. In the Path selection area, select the line. The preview of swept is visible in the design window. Set the thickness value 2mm and bend radius value 2mm. Click OK to execute the command. Change the colour of the model as according to your choice. Change the color of selected curved face of the model to distinguish it for Emboss text. Create a new sketch on this face. Activate the ‘Convert Entities’ command. Select the two vertical edges of the model. Create a horizontal line and apply dimensions. Activate the ‘Text’ command and select the line. Write the text as ‘Square Bend Tube’ and format the text. Click OK to create the text. Choose the Isometric View. Activate the ‘Wrap’ command, select the horizontal line which is based on the text. And select this face for wrap the text. ‘Emboss’ option is preselected, if you want to engrave the text you choose ‘Deboss’ option. You may also change height of embossed text. Click OK to execute the command. Change the color of face for good looking. In the same manner, emboss the text opposite side of the model. Save the Part file.
Ball Bearing || Autodesk Inventor Tutorial
In this Autodesk Inventor tutorial, we will learn about modelling a ‘Ball Bearing’ Assembly. The assembly has four components and a standard part. Four components will be created individually, later all of them will be placed into the assembly. So viewers will be able to watch part modelling as well as assembly modelling techniques of ‘Autodesk Inventor’ software. ………………………………………………………………………… The model designing concept is taken from videos available on YouTube. ………………………………………………………………………… Visit the following link to get the model file… http://bit.ly/2NsnVXP …………………………………………… Visit the following link to watch the basic tutorial on Autodesk Inventor by us https://www.youtube.com/playlist?list=PLb-IhKRMYSERYpB48aY-sZ10fN6CfXIL4 ………………………………………………………………. To watch detailed tutorials on the same software visit the following link https://www.youtube.com/playlist?list=PL74BDF7431ED13443 ……………………………………………………………………………… 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 us to get latest updates about our new uploads. http://www.youtube.com/user/nisheethsorjm?sub_confirmation=1
