Animation displayed in ‘Combination Pliers’ Assembly–SolidWorks 2014 (with caption and audio narration)
Serial No. 33 Animation displayed in ‘Combination Pliers’ Assembly–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 ‘Combination Pliers’, please visit on my another associated video named as ‘Combination Pliers’ (Video Tutorial) SolidWorks. Click the following link to get the model file: – http://bit.ly/2oyA2ti Transcription of the Video Create a new assembly inside an English template. The ‘Begin Assembly’ command is preactivated in the assembly design window. Place the ‘Part1’ file in the assembly. When the first part file is placed in the assembly, the part remains as a grounded component. So we will do unground the part with the help of ‘Float’ option. Right-click on the ‘Part1’ file and choose ‘Float’ option. Rotate the part by using ‘Move with Triad’ command. Save the assembly, name it as ‘Combination Pliers with Animation’. Select the part file in the design window and choose ‘Edit Part’ option. Go to the design tree, open the visibility of ‘Axis1’ and go on the ‘View’ tab and turn on the ‘Axes’ button. The Axis is shown in the design window. Return back to the assembly environment. Apply a ‘Coincident’ mate between the Top Plane of Assembly and Top Plane of ‘Part1’. Apply another ‘Coincident’ mate between the Axis1 of ‘Part1’ and Origin point of the Assembly. Activate the ‘Insert Component’ command, place the ‘Part2’ file in the assembly. Apply a ‘Concentric’ mate between the two holes of the Part. Apply a ‘Coincident’ mate between the inside face of the slot of ‘Part2’ and inside face of the slot of ‘Part1’. Drag the Plier to see the effect, the part moves on its own axis. Place the ‘Part3’ file in the assembly. Select the ‘Part3’ file and rotate to the proper position. Apply a ‘Concentric’ mate between inside cylindrical face of ‘Part3’ and inside cylindrical face of the hole of ‘Part1’. Apply a ‘Coincident’ mate between inside face of the ‘Part1’ and back face of ‘Part3’. Close the visibility of ‘Axis1’. Go to the View tab and turn on the ‘Planes’ button. Open the visibility of Right Plane of the assembly. Apply an ‘Angle’ mate on this face and Right Plane of the assembly. Set the angle value 0 degree and click OK. In the same way, apply another ‘Angle’ mate on the opposite side of the part. Apply a ‘Coincident’ mate between Right Plane of the ‘Part3’ and Right Plane of the assembly. Go to the ‘Mates’ folder and Suppress the ‘Angle2’ mate. Activate the ‘Move Component’ command and select the ‘Collision Detection’ option. Drag the part until touch to the opposite part. Now highlighted face shows here to stop the motion of the component at the moment of touch of any other entity. Click OK to finish the command. Go to the ‘Evaluate’ tab, measure the angle between these two edges of the part by using ‘Measure’ command. Activate the ‘Interference Detection’ command and check interference between the two components. Unsuppress the ‘Angle2’ mate. Go to the ‘Motion Study’ tab and click on the ‘Disable Playback of View Keys’ option on the animation timeline. Go to the Mates folder, select ‘Angle1’ mate and drag the timebar at 10 second. Modify the ‘Angle1’ mate key, fill the angle value to 20.077055 deg. and click OK. Drag the timebar at 13 second and right-click on the timeline, click ‘Place Key’ option. Pause the animation for 3 seconds. Drag the timebar at 23 second, double click on the ‘Angle1’ mate and fill the value 0 deg. in the Modify dialogue box, click OK. Repeat same steps which were done earlier for creating the animation of ‘Angle2’ mate. Click the ‘Collapse Motion Manager’ button. Now start the animation to see the result. Save the assembly.
Animation displayed in Box (mini size) — SolidWorks 2017 (with caption and audio narration)
Serial No. 215 Animation displayed in Box (mini size) — SolidWorks 2017 (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 in SolidWorks 2017. Click the following link to get the model file: – http://bit.ly/30MboTG Transcription of the Video Create a new assembly with an inch template. And place the ‘Part1’ file in the assembly. When the first part file is placed in the assembly, the part remains as a grounded component. This part does not need to place any mates. Go to the ‘View Orientation’ tab and choose an ‘Isometric’ view. Activate the ‘Insert Components’ command and place the ‘Part3’ file in the assembly. Apply a ‘Coincident’ mate between the Front face of ‘Part1’ and Back face of ‘Part3’. Apply a ‘Coincident’ mate between Front Plane of the assembly and Front Plane of ‘Part3’. Apply a ‘Distance’ mate between the top face of ‘Part3’ and ‘Part1’. Set the distance value 0.688 inches and click OK. Activate the ‘Insert Components’ command and place the ‘Part6’ file in the assembly. Apply a ‘Concentric’ mate between the inner circular face of ‘Part6’ and an outer circular ring of ‘Part1’. Apply a ‘Coincident’ mate between the back face of ‘Part1’ and back face of ‘Part6’. Save the assembly with the name ‘Base Assembly’. Apply a ‘Distance’ mate between the side face of ‘Part1’ and ‘Part6’. Set the distance value 2.564 inches and click OK. In the same manner, place a copy of ‘Part6’ in the assembly and mate it with ‘Part1’. Create another new assembly and place the ‘Part2’ file in the assembly. Open the visibility of Front Plane of assembly and turn on the ‘View Planes’ button. Open the visibility of Top Plane of ‘Part2’. Right-click on the ‘Part2’ file and select ‘Float’ option. Apply a ‘Coincident’ mate between the Top Plane of ‘Part2’ and Front Plane of Assembly. Turn off the visibility of planes. Apply a Coincident mate between Right Plane of ‘Part2’ and Right Plane of ‘Assembly2’. Save the assembly, name it as ‘Lid Assembly’. The part is not fully defined in the assembly, so that apply another ‘Coincident’ mate between the Top plane of Lid assembly and the Front plane of ‘Part2’. Activate the ‘Insert Components’ command and place the ‘Part7’ file in the assembly. Apply a ‘Coincident’ mate between the top face of ‘Part2’ and back face of ‘Part7’. Apply a ‘Coincident’ mate between Front Plane of Lid assembly and Front Plane of ‘Part7’. Apply a ‘Coincident’ mate between Right Plane of the ‘Part7’ and Right Plane of ‘Lid assembly’. Place the ‘Part5’ file in the assembly. Apply a ‘Concentric’ mate between the outer circular face of ‘Part5’ and inside face of the hole of ‘Part2’. Apply a ‘Coincident’ mate between Front Plane of ‘Part5’ and Front Plane of ‘Lid Assembly’. Apply a ‘Coincident’ mate between Right Plane of ‘Lid Assembly’ and Right Plane of ‘Part5’. Now the part is Fully Defined in the assembly. Go to the ‘Evaluate’ tab and check the interference between two components by using ‘Interference Detection’ command. Save and close all the assembly files. Create a new Assembly file, it is our main assembly to create animation, and place the ‘Base Assembly’ file in the assembly. Choose an Isometric View, right-click in the design area and activate the ‘View Orientation’ command. In the Orientation dialogue box, select the ‘New View’ option. Set the ‘Named View’ as ‘View-1’ and click OK. Save the assembly by the name ‘Box (mini size) with Animation’. Activate the ‘Insert Components’ command and place the ‘Lid Assembly’ file. Apply a ‘Concentric’ mate between inside hole of the hinge and outer circular face of wire. Apply a ‘Coincident’ mate between the side face of the hinge and face of slot of lid. Drag the Lid Assembly and see the result, the ‘Lid Assembly’ rotates on the base of the hinge. Place the ‘Part4’ file in the assembly. Apply a ‘Concentric’ mate between the hole of the ‘Part4’ and outer circular face of wire. Apply a ‘Coincident’ mate between the side face of ‘Part4’ and face of slot of lid. Apply a ‘Tangent’ mate between the bottom face of the lid and outer circular ring of ‘Part1’. Apply a ‘Coincident’ mate between the front face of ‘Base Assembly’ and back face of ‘Part4’. Place the ‘Part8’ file in the assembly. Turn off the visibility of the sketch of ‘Part8’ by using ‘View Sketches’ command. Apply a ‘Concentric’ mate between ‘Axis1’ of the Lid assembly and circular face of ‘Part8’. Apply a ‘Coincident’ mate between the Front Plane of ‘Part8’ and Front Plane of main assembly. Apply a ‘Tangent’ mate between the cylindrical face of ‘Part8’ and the top face of ‘Part7’. Check the interference between Handle and base. Suppress the ‘Tangent1’, ‘Coincident3’ and ‘Tangent2’ mates. Apply an ‘Angle’ mate between the Right Plane of ‘Part8’ and the top face of ‘Part7’. Set the angle value to 12.46923 degrees and Click OK. Change the name of the angle mate as ‘Drive-1’. Unsuppress the ‘Tangent1’ mate and apply an ‘Angle’ mate between the back face of the ‘Part4’ and the front face of the ‘Part1’. Set the angle value to 0 degree and Click OK. Change the name of the angle mate as ‘Drive-2’. Suppress the ‘Tangent1’ and ‘Drive-2’ mates. Drag the ‘Lid Assembly’ and turn on the ‘View Planes’ button. Apply the ‘Angle’ mate between Plane3 of ‘Part1’ and back face of ‘Lid Assembly’. Set the angle value to 0 degree and Click OK. Unsuppress the ‘Drive-2’ mate and change the name of the ‘Angle6’ mate as ‘Drive-3’. In the next section of this video, we will create three additional views with in alternate position of this model before entering the ‘Motion Study’ environment. These saved views will be used later in animation timeline. Click on the ‘Motion Study’ tab and click the ‘Collapse Motion Manager’ button. Choose ‘View-2’ in the Orientation
Carb Intake Plate — Autodesk Inventor 2018 Tutorial (with caption and audio narration)
Serial No. 291 Carb Intake Plate — Autodesk Inventor 2018 Tutorial (with caption and audio narration) Hello viewers in this tutorial we are going to create a model named ‘Carb Intake Plate’. This component is used in the assembly of ‘Carb’. ‘Carb’ is used as the subassembly in ‘Engine MKII’ model with 2 Clutch Shoes provided by the Autodesk Inventor software as the sample file. Click the following link to get the model file: – http://bit.ly/2o4EQGy Transcription of the Video Create a New part file with Inch units. Create the sketch over the XY Plane. Create a center point rectangle, coincident with the sketch origin. Apply 0.55 inches of dimension on its two sides. Apply fillets of 0.083 inches on all the four corners of the rectangle. Finish the sketch and activate the Extrude command, set the value of extrusion to 0.0625 inches next click OK. Change the Lightning in the file, here we are importing a customized settings which we saved earlier. Change the colour of the model as per your wish so that it looks good. Save the file with the name Carb Intake Plate. Now create a sketch on the front face of the model. Take the project of this face of the model by using the Project Cut Edges command. Convert projected edges into the construction geometry. Select four center points of the arc and convert it to center point. Activate the Hole command, you can see here all the four points will be selected automatically, that were converted into center point earlier. Fill the diameter of holes 0.1 inches and through all in termination field. Click Ok to create the hole. Turnoff the shaded view. Create a work plane, -0.15 inches away from this face of the model. Draw a sketch on this plane. Activate Slice Graphic command and take the project of intersecting edges of the model. Convert all the projected edges into construction geometry except following one. Draw a line 0.25 inch offset from this line next add two more lines to create an a closed profile. Add another line and add a coincident constraint between the midpoint of this line and end point of this line. Convert this line into construction geometry. Apply the angular dimension of 45° between these lines. And exit from the sketching mode. Create another work plane similar to the last one on the opposite side. Activate the Extrude command sketch will be selected automatically, in the Extents field select ‘To’ option and select this work Plane. Click Ok to create extrude feature. Close the visibility of open work planes. Apply a fillet of 0.125 inches on these two corners of the model. Turnoff the textures to see the model clearly. Create a hole on following face of the model. Fill 0.15 and 0.125 inches in linear offset distance after defining the reference edges. Fill the diameter of the hole 0.1875 and 0.3 inches in depth field. The file is complete so save it.
Engine Piston — Autodesk Inventor 2016 Tutorial (with caption and audio narration)
Serial No. 226 Engine Piston — Autodesk Inventor 2016 Tutorial (with caption and audio narration) The Design of ‘Engine Piston’ 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 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=PLKWX3xUP3pPp1ndQrE1t73DCTp-W4ZWLd Click the following link to get the model file: – http://bit.ly/2nSHfnE Transcription of the Video Create a new inch part file. Activate the Extrude command and create a new sketch over the XY plane. Create a circle of 0.551 inch diameter coincident from the origin. Finish the sketch, set the value 0.375 inch of extrusion and click OK. Fill the name of the file ‘Engine Piston’ and save it. Create a sketch on this face, take the project of the circle by using ‘Project Geometry’ command. Create a center point rectangle which is coincident with the center point of circle. Draw the two arcs and apply the dimensions. Add the equal and concentric constrain to get the sketch fully constrained. Activate the Extrude command, select the profile and choose ‘Cut’ option and set the depth value, click OK. Create a sketch on this face, take the project of part face by using ‘Project Geometry’ command. Choose slice graphics option, take the offset outside of the circle and set dimension value. Draw two lines between endpoint of tangent arc and line. Convert this circle into construction geometry and create another 3point arc to close the profile. Finish the sketch, select the profile and extrude it 0.0925inch, click OK. Now see, add another extruded feature has been created, which was made by the ‘Join’ operation earlier. Activate the ‘Mirror’ command select the extruded feature and choose mid plane, click OK. Activate the Fillet command, the fillet select mode type as feature select any one edge of the inside of part, it will be automatically selected all inside edges and apply it. Here three types of selection mode are available, any option can be selected as you need according to your design. Click Ok to create the fillet. The file is complete and save it.
Front Axel — Autodesk Inventor 2016 Tutorial (with caption and audio narration)
Serial No. 289 Front Axel — Autodesk Inventor 2016 Tutorial (with caption and audio narration) The Design of ‘Front Axel’ has been taken from Assembly file of ‘Suspension’ → ‘Sample files’ → Autodesk Inventor.Rest components of the model ‘Suspension Assembly’ (consisting in several numbers) have also been designed. You may watch them by visiting on following playlist:- https://www.youtube.com/playlist?list=PLKWX3xUP3pProQ20K3hW-qxzjEMXjaq-R._________________________________________________________Inside this video, you can see full detailed process of making 3-D Parametric CAD Model through Autodesk Inventor Software. Click the following link to get the model file: – http://bit.ly/2o8eyTO Transcription of the Video Create a new inch part file. Create a new sketch over the XY plane. Create a circle with specified diameter and coincident from the origin. Finish the sketch and activate the Extrude command. Click ‘Direct 2’ button to reverse the direction of extrusion and set the pre decided value of extrusion and click OK. Save the file with the name ‘Front Axel’. Create a new sketch on this face, take the project of the circular edge by using the ‘Project Cut Edges’ command. Create a new circle with required dimension. Activate the Extrude command, select the region and apply the suitable distance value, click ‘More’ option, set taper angle to -40 degree and click OK. Create a new sketch over the YZ plane. Take the project of the model by using the ‘Project Cut Edges’ command. Project Cut Edges command helps to provide all the edges of model, intersecting the active sketch plane in the current sketch. You can draw the sketch like line, arc, circle etc., easily snapping on the model edges. Now the sketch is complete, so finish the sketch and Activate the ‘Revolve’ command, select the two regions and select the center line as an axis of revolution. Click OK to create the revolve feature. Apply the fillet on four inside edges of the part. Activate the Extrude command and create a sketch on this face. Draw a circle and take project of this edge. Apply the distance value, click OK to execute command. Apply the Chamfer on these two edges and click OK. Go on the browser bar and open the visibility of Sketch3. Activate the Work Point command. Go on the view tab, change the visual style of a model as a Wireframe. Click on the center point of arc, now the work point has been created. Close the visibility of the sketch. Return to the ‘Shaded with Edges’ view. Activate the Work plane command and select this work point in browser bar, select this face. Now see here a Work plane is created on this work point. Create a new sketch on this plane. Activate the slice graphics command. Take the project of YZ and XZ plane by using the ‘Project Geometry’ command. Draw a rectangle and apply coincident constraint between midpoint of the rectangle and center line. Draw an arc, which is tangent to this rectangle and apply the required dimensions. Finish the sketch and activate the Revolve command. It will be automatically select the profile, select the center line as an axis of revolution, select ‘Cut’ operation and click OK. Repeat this revolve cut feature to create on opposite side of the part by using the ‘Mirror’ command. Create a sketch over the YZ Plane. Take the project of this work point and draw a circle with required dimension. Finish the sketch and activate the ‘Extrude’ command. Choose the ‘Cut’ operation and select ‘Symmetric’ option, select ‘All’ option in the ‘Extent’ field to cut the hole through all body. Click OK to create Extruded Cut feature. Apply the Chamfer on these two edges of the part. Create another hole by using ‘Extrude’ command as previously done. Activate the ‘Thread’ command and select this cylindrical face and give the specifications of the thread as per need to our design. Change the color of the model as per your wish so that it looks good. Save the file.
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
Box (mini size) supported with Animation (Solid Edge ST9) with caption and audio narration
Serial No. 40 Box (mini size) supported with Animation (Solid Edge ST9) with caption and audio narration……………………………………………………………….In this video, we will display how to create an animation of our model ‘Box (mini size)’ using ‘Simulate Motor’ command. In this model we have created two subassemblies, one is ‘Base Assembly’ & other is ‘Lid Assembly’ by using Assemble command. ………………………………………………………………………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/2OuEHaM Transcription of the Video Create a new inch assembly file. Save the file, name it as ‘Base Assembly’. Activate the ‘Insert Component’ command. Go to the ‘Parts Library’ tab and browse the folder ‘Box (mini size) with Animation’. Place the ‘Base Body’ part file in the assembly. Activate the ‘Insert Component’ command. Place the ‘Hook of Latch’ part file. ‘Assemble’ command is pre-activated by default when the part is placed in the assembly. Select the back face of Hook of Latch and the front face of the Base Body and apply the mate. Activate the ‘Assemble-Construction Display’ command. And choose ‘Show Reference Planes’ option. Open the visibility of reference planes of assembly. Apply a mate between the right plane of Hook of Latch and Base Body. Activate the ‘Planar Align’ command and set the offset value 0.688 inch. Apply a Planar Align mate between the top face of hook and base. Close the visibility of reference planes of assembly. Place the part file ‘Hinge’ and apply an axis mate between the inner circular face of Hinge and outer circular face of the base. Click ‘Flip Side’ button to rotate the part. Activate the ‘Flash Fit’ command, select the back face of Hinge and Base body and choose the flip side button to apply mate. Apply the Planar Align mate between Hinge and Base Body and set the offset value 2.564 inch. In the ‘Assemble’ command, ‘Flash Fit’ option is very useful tool in this software, for mating the assembly components easily in the assembly environment. This tool reduces the number of steps of the assembly relationships (like Mate, Planar Align and Axil Align mates etc.) In the same manner, fix one more Hinge on the Base Body. Open a new subassembly and place the Lid part file. Save the assembly, name it as ‘Lid Assembly’. Place the ‘Handle Base’ part file by using ‘Assemble’ command. Apply the mate between the back face of Handle Base and top face of Lid. Go to the Assemble tab and choose ‘Show Reference Planes’ option. The Planes of Handle Base are visible in the design window. Open the visibility of assembly planes. Apply the mate between the Right plane of Handle Base and Lid. Apply another mate between Front Plane of Handle Base and Lid. Close the visibility of all visible planes. In the same manner, place the ‘Wire’ part in the assembly and apply the mate. Go to the Inspect tab and check the Interference between ‘Wire’ and ‘Lid’ components by using ‘Check Interference’ command. Save the file and close all the subassemblies. Create a new inch assembly, this is our main assembly. Base Assembly and Lid Assembly will be placed in this assembly which has been created earlier. Save the file with the name ‘Box (mini size) with Animation’. Apply the Mate between the outer circular face of Wire and inner circular face of Hinge. Apply another mate between inner slot face of Lid and the front face of Hinge. Now drag the Lid subassembly by using ‘Drag Component’ command. The Lid Assembly starts to move on the base of Hinge. Check the Interference between ‘Lid Assembly’ and ‘Base Assembly’. Apply a tangent mate between the bottom face of Lid and cylindrical face of the Base Body part. Place the ‘Handle Wire’ part file. And select it, choose the Show/Hide Component option. Place the checkmark in the ‘Reference Planes’ On button and click OK. Close the visibility of Base assembly. Open the visibility of Right plane of Lid Assembly. Apply a Mate between the Right planes of Lid Assembly and Handle Wire. Apply a Connect mate between the axis of Handle Wire and the Front plane of Lid Assembly. Apply another Connect mate between the axis of Handle Wire and Plane 4 of Handle Base. Hide all the work planes in the assembly by using Show/Hide Component command. Rotate the handle to the proper position by using ‘Drag Component’ tool. Place the part file ‘Top of Latch’ in the assembly. Apply the mate constraint between Axis of Top of Latch and Wire. Apply another mate between the side face of Latch and inner slot face of Lid. Activate the ‘Angle’ mate command → select the front face of the latch → select the front face of the lid, and at last select side face of the lid and apply the mate. Select the Top of Latch part and set the angle mate value to 0-degree, click accept. Apply a Tangent mate between Handle Wire and the top face of Handle base. Three mates such as angle mate of Top of Latch, Tangent mate of Handle Wire and Tangent mate of Lid Assembly have to be Suppressed before going in the motion environment. Activate the ‘Rotational Motor’ command. ‘Select Moving Part Step’ option is preselected. Select the ‘Handle Wire’ part as moving part. Choose the ‘Select Axis Step’ option. Select the cylindrical face of ‘Handle Wire’, the part will rotate about the axis. Use the ‘Flip Direction’ button in reverse direction. Set the speed of motor 20 degree/sec and set the Limit value to 165.64 degrees. In the same manner, set the motor on the ‘Top of Latch’ and ‘Lid Assembly’ by using ‘Rotational Motor’ command. Now see in the browser bar, three Rotational motion is visible under the Motors folder. Go to the Tools tab → ‘Environs’ panel and activate the ‘Explode-Render-Animate’ command. Activate the ‘Animation Editor’ command, the animation
