Photo Frame (Design-1)–Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 206 Photo Frame (Design-1)–Autodesk Inventor 2013 (with caption and audio narration) This video tutorial features the designing process of a Photo Frame with the aid of Autodesk Inventor’s part and assembly modelling functionality. The highlight of the video is application of ‘Copy Components’ feature that is quite a time saving utility available in the Assembly modelling environment. Click the following link to get the model file: –http://bit.ly/2osKeUj Transcription of Video Create a new Part file with an English template. Create a new sketch on the XY Plane. Create the base sketch of photo frame with the given dimensions and by utilizing line tool. The sketch is complete. Exit from the sketching environment. Activate the Extrude command from the marking menu. In the Extrude dialogue box, select ‘Symmetric’ option for the direction. Enter the value in the distance field and execute the command. Change the model colour to Flaked Reflective Beige. Pick the ‘Angle to Plane around Edge’ tool. Click the left vertical edge of the model and then select front face of the model. Enter the angle in the edit box. Click the green check mark to create a work plane for the new location. Create a new sketch on this plane. Use the Projected cut Edges tool to get the projected edges of the model. Finish the 2D Sketch. Activate the Extrude command to remove the side portion of the model. Close the visibility of this work plane. Apply the same type of cut feature on the opposite side of the model by using Mirror tool. Activate the Mirror tool and select Extrusion1 from browser bar. Select XY Plane of the model as a reference plane for the mirror. Click OK to create the mirror feature. Save the part file with its default name. Close the part file. Create a new Assembly file with an English template. Place the Part1 file by utilizing ‘Place Component’ tool. Save the assembly file with the name ‘Photo Frame (Design-1)’. Activate the ‘Copy Components’ tool. Copy Components dialogue box is displayed in the graphics window. Select the Part1 file in the graphics window. Blue double plus status button is selected by default. This button indicates; the newly generated component will be saved in a separate part file that will not be associative to the source part file. Click Next button. Uncheck the ‘Suffix’ option in the Naming Scheme section and apply it. Change the name of file Part2. Click OK to close the dialogue box. Edit the Part2 to resize the model. Unground the Part2 to apply the constraints. Rotate the Part2 by using Rotate Component tool. Apply Mate constrain between side faces of both parts. Apply another Mate constrain between two vertical edges of both parts. Apply Flush Mate between top faces of both parts. Check the interface between two parts. Activate the ‘Copy Components’ tool again. Activate the ‘Suffix’ option in the Naming Scheme section and apply it. Change the grounded position of the newly created copy of the Part 1. Rotate the component to properly position it for applying new mates. Apply the same set of mates as shown earlier. Now create a copy of Part 2 in the assembly and properly position it. Apply mates between the components to complete the model.
Modelling an Elbow in Creo Parametric 2.0
In this tutorial we will create an Elbow by utilizing part modelling capabilities of Creo Parametric 2.0 Viewers will be able to watch application of many part modelling tools like Sweep, Shell, Helical Sweep, Pattern and Round tool as well as 2D sketching techniques are also shown. In cutting of threads I will utilize the same BSP Thread Profile that was shown a previous video by me.. Video Screen Shots View Full Album Transcription of Video Start a new part file from scratch with the default template and give it a name ‘Elbow’. Select the Top Datum plane and create a new sketch on this plane. Click the Sketch View icon to orient the sketching plane parallel to the screen. Clear the screen by closing the visibility of Datum Planes, Axis, Points, Spin centre, etc. Activate the line tool and draw the sketch as displayed. As soon as the lines are drawn the constraints are automatically applied. Change the dimension values as displayed. Activate the Circular Fillet tool and apply a fillet between these two lines. Fill the radius of the fillet. Select the dimensions and lock them. The sketch is complete so exit from the sketching mode. Activate the Sweep tool. Define the visible sketch as trajectory for the sweep. Flip the direction of the sweep. Click this icon to activate internal sketcher for creating the sweep cross section. Draw a circle at the end of trajectory and apply the dimensions as displayed. Click Ok to return to the Sweep tab. The preview of the feature is visible so click ok to execute the command. Change the colour of the model as per your wish. Activate the Shell tool. Select the surfaces of the model to be removed. Use ctrl key of your keyboard while selecting multiple surfaces. Specify the Shell thickness and execute the command. Save the model file. Open the visibility of datum planes and create a sketch over Top datum plane. First create a centerline in the sketch that will work as axis of revolution for the sweep. Take the project of the internal edge of the model. Delete this line. You can see a reference line still exists which will be used to create a new line for Helical sweep profile. Fill the dimension value which will be the length of thread. Exit from the sketching mode. Open the file named ‘BSP_Thread_Profile’. Here you can see a sketch profile of a British Standard Pipe Thread is drawn. The pitch of the profile is 1/14 inches which governs all the other dimensions by some relations. Copy this sketch profile. Now switch back to Elbow file. Activate the Helical Sweep tool. At present software prompts to select an open sketch to define Helix sweep profile so select this line. Fill the pitch value as displayed. Click this icon to create the sweep section or profile. Place a geometry point. Now paste the BSP Thread Profile that was copied earlier and which is still in the Windows Clipboard. As soon as you paste the sketch the move tool will activate. In the scale field fill the value 1. Rotate the profile by 90° in clock wise direction. Move the profile near to the geometry point and click Ok. Make some minor correction in the profile because in pasting it some constraints have gone missing. Again move the profile more near to the geometry point to apply some more constraints. Delete any constraint that gives error in placing new constraint. Now profile is properly positioned so exit the sketch. The preview of sweep is visible in the graphic window. Activate the remove material option and execute the command. Activate the shaded with edges option. Hide the visibility of visible sketch. Select the Helical sweep in the Model Tree and activate the Pattern Tool. Open the visibility of Coordinate System. Set Axis as the type of pattern. Select Y axis of Coordinate System as axis of rotation. Enter the number of members to be patterned. Define the Angle between the pattern members. Execute the command. Activate the Round Tool. Fill the radius of round. Select the edges and execute the command. The fully created model is in front of you. Switch between the Shading With Edges and Shading view. Save the model file. Get the Model file by visiting the following link:-http://bit.ly/2m7Haw4
Thread Cutting in Bolt & Nut-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 205 Thread Cutting in Bolt & Nut-Autodesk Inventor 2013 (with caption and audio narration) In this video tutorial we will show how to create a thread on a nut and bolt by using a thread profile and applying the coil tool in Autodesk Inventor. In our previous video we displayed how to create a sketch profile of a Unified and American screw (internal). We will utilize the same sketch profile here. Click the following link to get the model file: – http://bit.ly/2nI85Pq Transcription of Video Open the file of Bolt. Start a new sketch on YZ plane of the part. Activate the Slice Graphics Command. This will slice away the portion of the model temporarily that hides the plane on which we want to sketch. Take the project of the model by activating the Project Cut Edges tool and convert them to the construction geometry. Now draw a rectangle as shown and apply a construction override on it. Open the file named Unified and American screw external thread. Select the sketch profile drawn in the file and copy it as displayed. Switch back to the Bolt file and paste it on the sketch. Add a line to close this profile. Rotate this profile 90° in a clockwise direction by utilizing the Rotate Tool. Pick up the Move tool and place the profile on a new location. Snap it to this point of rectangle. Finish the sketch and activate the coil tool, it will automatically select the thread profile. Next define the Z axis of the model as the Axis for the thread cutting. Switch to Coil Tab of the tool dialogue box and set the type of the coil to Pitch and Height. Fill the values in the Pitch and Height input boxes. Switch back to the Coil Shape Tab and Select the Operation Type to Cut. Click Ok to execute the command. Start a new sketch over YZ Plane. Take the project of the constructed part and take the measurement between the two threads to check the pitch created by coil tool. Exit from the sketch and close its visibility from the browser bar. Save the file and close it. Open the file of Nut. Start a new sketch over the back face of the model. Select the projected centre point of the model and convert it to centre point. Exit the sketch and activate the hole tool. It will automatically select the placement point of the hole because we applied a centre point override over the projected centre point of the part in our previous sketch. Set the type of the hole to Tapped Hole. Define the setting of the hole as displayed and execute the command. Check the diameter of the hole by utilizing the measure tool. Now select the hole feature in the browse and edit it. Set the type of the hole to simple hole and execute the command. Activate the chamfer tool. Set the type of the chamfer to distance and angle. First select the back face from which the chamfer is angled and then select this edge of the hole. Fill the values in distance input box and leave the default angle value unchanged. Click Ok to execute the command. Start a new sketch over YZ Plane. Activate the slice graphics command and the project of the model edges. Convert all the lines into construction line. Open the file named Unified and American screw external thread. Select the sketch profile drawn in the file and copy it as displayed. Switch back to the Nut file and paste it into the sketch. Add a line to close this profile. Rotate this profile 90° in a clockwise direction by utilizing the Rotate Tool. Now draw a rectangle as shown and apply a construction override on it. Pick up the Move tool and place the profile on a new location. Measure the length of the Nut. Activate the coil tool from the right click context menu, it will automatically select the thread profile. Next define the Z axis of the model as the Axis for the thread cutting. Switch to Coil Tab of the tool dialogue box and set the type of the coil to Pitch and Height. Fill the values in the Pitch and Height input boxes. Switch back to the Coil Shape Tab and Select the Operation Type to Cut. Next execute the command. Start a new sketch over YZ Plane. Take the project of the constructed part and take the measurement between the two threads to check the pitch created by coil tool. Exit from the sketch and close its visibility from the browser bar. Save the file.
Hem Tool-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 204 Hem Tool-Autodesk Inventor 2013 (with caption and audio narration) Hem tool is used to strengthen or eliminate sharp edges of the sheet metal face. You can create single, double, rolled and teardrop hems. This tool is available on Create panel of sheet metal Tab. Click the following link to get the model file: – http://bit.ly/2nJxFnj Transcription of Video 1. Open the Assembly file of ‘Chassis for Constant Voltage Transformer’. 2. In the Browser Bar double click the ‘Part3′ file to edit it. 3. Go to the ribbon, Create panel > Hem tool. 4. The Hem dialogue box is visible in the design window. 5. In the Shape tab, the Edge Selection button is active. 6. Select the left inside vertical edge of the sheet. 7. The preview of Hem is displayed in the design window. 8. Fill the values in the ‘Gap’ and ‘Length’ input box as displayed. 9. Click OK to create new hem. 10. Return back to the assembly environment. 11. Mirror of Part3 is automatically updated. 12. In the Browser Bar, double click the ‘Part4′ file to edit it. 13. Repeat the same steps and apply two more hem features on the left and right inside vertical edges of the sheet. 14. Reactivate the hem tool and select top inside edge of the sheet. 15. Click more button to expand the dialogue box. 16. By default, ‘Width Extents’ Type ‘Edge’ is selected. 17. Change it to ‘Offset’. 18. In the ‘OffSet1’ input box, expand the node to activate the Measure tool. 19. Select the left face of the sheet and right face of the hem. 20. The distance between the two faces will be added in the offset input box. 21. In the similar way add values in the ‘OffSet2’ input box. 22. Switch to the Bend tab, change the ‘Relief Shape’ type to ‘Tear’. 23. Click OK to execute the command. 24. At the end, remove the remaining extended faces by using Cut tool. 25. Open the Part4 file separately, to check the Flat Pattern of the sheet.
Face tool and Flange tool-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 203 Face tool and Flange tool-Autodesk Inventor 2013 (with caption and audio narration) Click the following link to get the model file: – http://bit.ly/2mVWsV4 Transcription of Video Face Tool is used to create sheet metal faces by utilizing a closed sketch profile. It is similar to extrude tool where height is automatically set to the thickness of the sheet. This tool is available on the Create panel of Sheet Metal Tab. 1. Open the Assembly file of ‘Chassis for Constant Voltage Transformer’. 2. In the Browser Bar double click the Part2 file to edit it. 3. A closed sketch profile is previously created in Sketch1 of this file. 4. Go on the ribbon, Create panel > Face tool. 5. The Face dialogue box is visible in the design window. 6. The rectangular profile is automatically selected in the design window. 7. Click the ‘Flip Offset’ button to change the direction of the extrusion. 8. And click OK to create sheet metal face. Flange Tool is used to add a sheet metal planer face and a bend on an existing sheet metal edge. The depth and the angle of the flange can be specified. This tool is available on the Create panel of Sheet Metal Tab. 1. Rotate the model by using View Cube. 2. Go on the ribbon, Create panel > Flange tool. 3. The Flange dialogue box is visible in the design window. 4. In the Shape tab there are two options for creating a flange, first option is ‘Edge Select Mode’ and the other is ‘Loop Select Mode’. 5. Currently the Edge Select Mode button is active allowing you to select only one edge at a time. 6. Select four inside edges of the sheet one by one. 7. Delete the selections and try next option. 8. Click the ‘Loop Select Mode’ button, so you can select multiple edges at a time. 9. By default, ‘Inside of bend face’ option is selected as the ‘Bend Position’. 10. Change it to ‘Outside of base face’. 11. Fill the value in the Height Extents field. 12. Click OK to create new flange.
Punch Tool-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 202 Punch Tool-Autodesk Inventor 2013 (with caption and audio narration) The Punch Tool command is used to cut or deform sheets by placing predefined Punch tool geometry. To apply this tool the sheet metal face must have a sketch with one or more unconsumed centre mark. This tool is available on the Modify panel of Sheet Metal Tab. Click the following link to get the model file: – http://bit.ly/2onIxY5 Transcription of Video 1. Open the Part 1 file. 2. Start a sketch on the back face of the model to define centre marks for punch tool. 3. Place a centre point on the sheet and apply dimensions as displayed. 4. Duplicate this point 4 times by using Rectangular Pattern tool. 5. Activate the tool and select the centre point. 6. Define the direction of Pattern. 7. Fill up the occurrence count and spacing between the points. 8. Apply the command. 9. Exit from the sketching mode. 10. Activate the Punch tool from the Modify panel. 11. The PunchTool Directory dialogue box is displayed. 12. Manually locate Sheet Metal Punch iFeature file LouvrePunch and open it. 13. Punch Tool dialogue box is displayed and a preview of punche is visible. 14. Switch to Geometry tab and fill the value in the Angle field. 15. Next click the Size tab and change the values of Width, Length and Height one by one. 16. Click the Refresh button to update all the added values on-screen. 17. Click Finish in the Punch Tool dialog box to place the punches.
Chassis for Constant Voltage Transformer by Sheet Metal (Autodesk Inventor 2013)
Serial No. 190 Chassis for Constant Voltage Transformer by Sheet Metal (Autodesk Inventor 2013) Inside this video, viewers will watch full detailed process of creating this model through Autodesk Inventor Software’s Sheet Metal design functionality. Click the following link to get the model file: – http://bit.ly/2nD4jH4
Creating Relation Based Sketches in Creo Parametric 2.0 || British Standard Pipe Thread Profile
This tutorial will display how to create relation based sketches in Creo Parametric. As an example we will create a sketch profile of a British Standard Pipe Thread. The pitch of the profile is 1/14 inch. Transcription of Video Start a new part file from scratch with the default template and give it a name ‘BSP_Thread_Profile. You can see the English template is opened by default. Select the Front Datum plane and create a new sketch on this plane. Click the Sketch View icon to orient the sketching plane parallel to the screen. Clear the screen by closing the visibility of Spin centre, Datum Planes, Axis, Points etc. Go to setup panel and define the Grid settings. In the Grid setting dialogue box activate Static Grid spacing option and modify the X and Y spacing as displayed. Open the visibility of Grid from Sketcher display filters. Now zoom the window quite considerable to view the Grid. Draw a sketch with the help of line tool as displayed. You will see that some constraints are automatically applied and intimated time to time by the software. Create a centreline for our sketch. Apply dimensions related to our profile specification. Lock this dimension to preserve it from any modification. Again, apply an angular dimension. Apply constraints according to the demand of the sketch. Quit the sketching mode. Switch to Annotate Tab. Activate Show Annotation Tool and select the sketch. All the applied dimensions in the sketching environment will be visible. Terminate the command. Select this dimension in the design window that will be highlighted in Model Tree. Open its property from the context menu. Change its display name to ‘P’ and apply changes. Go to model Tab—Model Intent Panel and expand it to find Switch Symbol Command. Click it to display names of dimension in spite of values. Re-edit the sketch. Draw an arc tangent to both the lines. Define the Angular dimension and apply a Lock over this dimension. Exit the sketching mode and again redefine the names of the dimensions. Remove the Prefix otherwise dimension will display Rr name that will be very confusing. Expand the Model Intent Panel and Activate the Relation command. Start adding the values according to the profile. You can type or paste the values. Execute and verify the relations. Select the dimension of pitch with the help of selection filters easily. Move it to new location. Re-edit the sketch. Add more dimensions to the sketch and change its name. Give away relation according to the profile. Adding this dimension is conflicting with a previously placed constraint, so remove that constraint. Similar operations are being performed as done earlier. Again re-edit the sketch. Select these two lines and convert them to construction lines. Complete the sketch by adding few more arcs and lines. Select these sketches and duplicate using Mirror Tool. Now sketch is complete so finish the sketch and save the file. If you change the pitch, the profile will change simultaneously.
Chassis for Automatic Voltage Regulator by Sheet Metal (Autodesk Inventor 2013)
Serial No. 189 Chassis for Automatic Voltage Regulator by Sheet Metal (Autodesk Inventor 2013) Inside this video, viewers will watch full detailed process of creating this model through Autodesk Inventor Software’s Sheet Metal design functionality . Click the following link to get the model file: – http://bit.ly/2omQj4E
Circular Tub through Sheet Metal-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 188 Circular Tub through Sheet Metal-Autodesk Inventor 2013 (with caption and audio narration) Inside this video, viewers will watch the full detailed process of creating this model through Autodesk Inventor Software’s Sheet Metal design functionality. Click the following link to get the model file: – http://bit.ly/2nJu6gA Transcription of Video Create a new sheet metal part file with an English template. Go to Setup panel and activate Sheet Metal Defaults. Specify the thickness of the sheet manually and end the command. Create a new sketch over the XY plane. Take the project of Y Axis and convert this projected line into centreline. Draw a sketch along with dimensions by utilizing Line tool. Use constrains to position the geometry and fully constrain the sketch. The required sketch is complete, hence finish the sketch. Go to Create panel and activate Contour Roll tool. Profile geometry and rotation axis are automatically selected. Offset the material thickness to the other side of the selected profile. Fill up the Rolled Angle. Activate sweep the Contour Roll both side equally option. Terminate the command. Save the part file with the default name. Change the colour of the model to Flaked Reflective-Being. Activate Cross Section Analysis Tool to get the information about the interior of the part. This view provides a cutaway view of the part along XY plane. Now deactivate the command from the Browser Bar. Go to Flat Patten panel and activate Create Flat Pattern tool. Check the bend sequence of the part by activating the Bend Order Annotation command. Return back to folded Sheet Metal part. Save and close the file. Create a new assembly file with an English template. Place the previously created sheet metal part in the assembly. Save the assembly with the name ‘Circular Tub through Sheet Metal’. Create a new sheet metal part in the assembly using English template. Define XY Plane of the Assembly as the sketch plane for the base feature. Specify the thickness of the sheet by activating Sheet Metal Defaults command. Start a new sketch over the XY plane of the part. Take the project of Part 1 by using Project Cut edges command. Activate Project Geometry tool and take the project of Y axis. Convert all the projected lines into Construction Geometry. Finish the sketch and return back to assembly. Switch to View tab—Appearance panel and activate Half Section View along the XY plane of the assembly. Again edit the Part 2 and activate the previously created Sketch 1. Draw a sketch along with dimensions as displayed. The required sketch is complete so finish the sketch. Activate the Contour Roll tool. Profile geometry is automatically selected so define Y axis as axis of rotation. Offset the material thickness to both side of the selected profile. Activate sweep the contour roll both side equally option. The last applied Rolled Angle is filled up automatically. Execute the command. Change the colour of the part to Maple – Solid Natural Medium Gloss. Save the part file and return to assembly. In the assembly Half Section View is active, take a closer look of the assembly to get the information about the interior of the model. Switch to View tab and end the Half Section View command. Select the Part 2 in the browser bar and open it separately. Check the Flat Pattern of the model as well as Bend Order sequence. Close the part and return to assembly. At present there are degrees of freedom in the assembly. Apply a Mate constraint between Y Axis of Assembly and Y Axis of Part 2. Activate Flush Mate and click ‘Predict Offset and Orientation’ option. Select top face of Part 1 and top face of Part 2 and apply the flush mate. Now there is no degree of freedom left in the assembly. Switch to Inspect Tab and Analyze interface between the assembly parts. There were no interfaces detected. Save the file.
