Creating Lines in a 2D sketch in Autodesk Inventor 2013
Video Tutorial with caption and audio narration Transcription of Video Open a new standard (mm).ipt file from the scratch. To start a new sketch, click Create 2D Sketch icon present on the sketch panel of 3D Model Tab. Select any of the work plane to start the sketching. Select Front in view cube to adjust the design window. If your design window looks different change the settings of your software in following way. Click the Tools Tab and activate the Application Option Tool. General Tab is displayed by default. Now click the Sketch Tab. Make sure the settings of your software should be same as displayed here. Applying the setting and close the dialogue box. Now activate the sketch Tab to display the sketching tools. Line tool is located in Draw Panel of Sketch Tab. Click on its Icon to activate the tool. Click anywhere in design window to place a start point of the line and then click again to place the end point of the line. So in this way you can create a zigzag of lines. To draw a defined length of line you can take the help of heads up display. If heads up display is not enabled in your software you can turn it on from the Application option. You can control the settings of heads up display by clicking its setting tab. By the heads up display you can define a point’s X and Y location. You can also define the length and angle of a line. A dimension will be automatically applied when a dimension is filled. You can activate line tool even by marking menu. Click Tab key on your keyboard and fill 0 in the X input box. Click tab key again to switch to Y tab and fill the value 50. Click Enter key to place the start of line. Use tab key of your keyboard to switch between heads up input box and use enter key to place the points in the design window. With the help of Line Tool, you can even create Tangent Arcs.
Creating a new Part on the curve surface in Assembly-Autodesk Inventor 2013 (with caption and audio)
Serial No. 194 Creating a new Part on the curve surface in Assembly-Autodesk Inventor 2013 (with caption and audio) In this exercise, a pre constructed part file (Base) is utilized, which is taken from our model ‘Can’. Click the following link to get the model file: – http://bit.ly/2nO8BeB Transcription of Video We have following cylindrical component named ‘Base’ in our incomplete assembly. The target is to create and fix a ‘Clip’ on its cylindrical face. Now create a new component in the assembly with the name ‘Clip’. Select the Standard (in).ipt template for the new part file. Select the Centre point of the assembly as a base plane for the new component. Return back to the assembly environment by clicking Return icon. At present the part is not fully constrained in the assembly. Remove the degrees of freedom of the component (Clip) by applying Mate constraints. So, after applying the Mate constraints no degrees of freedom is left in the Assembly. Double click the Clip part to edit it. Create a new sketch on the XY Plane of the Clip. Take the project of base part with the help of Project Cut Edges tool. Convert all the sketches into construction geometry. Exit the sketching environment. Create a new Work Plane on this point, perpendicular to projected vertical line of the base part. Create a new sketch on this work plane. Take the project of base part once again. Exit the sketching mode and change the name of the sketch as ‘Base sketch of Clip’ in the Browser Bar. Again enter in the sketching environment. Draw the desired sketch with the aid of 2D sketching tools as displayed. Use the constraints to properly position the sketch. Convert unwanted sketches into construction geometry. Now our base sketch is complete. Finish the sketch and start a new sketch on the same work plane. Take the project of following intersection points and arcs of the sketch. Close the visibility of the base sketch to see the projected points and arcs clearly. Complete the sketch as displayed. Now our sketch is complete so exit the sketching environment. Extrude this sketch profile 5/8 inch in the downward direction. Change the colour of the Part to ‘Steel’. Return back to the assembly environment. Check the interference between the both parts with the help of ‘Analyze Interference’ tool that is available on the Interference panel of Inspect tab. Activate the tool, first select the Base part and then the Clip, click Ok to Analyze. There was no interference detected. Edit the Clip part once again. Create a new sketch on the front face of the Clip. And draw sketch profile as displayed. Extrude the sketch profile and select Cut option in the extrude dialog box. In the Extents field select ‘All’ from the drop down list to remove the material from the Clip. Mirror this extrude feature with the aid of Mirror tool. Select XY Plane of the Clip as mirroring plane. Now create a hole on the front face of the Clip. Hole should lie on centre of the front face. Now our model is complete.
Creating Tooth of Hacksaw Blade-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 193 Creating Tooth of Hacksaw Blade-Autodesk Inventor 2013 (with caption and audio narration) In this exercise we have used two 3D features → Extrude (Cut operation) and Rectangular Pattern. Here a pre constructed part ‘Blade’ is taken from the model ‘Hacksaw’. Click the following link to get the model file: – http://bit.ly/2ooUYmN Transcription of Video Open the Blade (.ipt) file. A pre constructed Blade part file is visible in isometric view. Select blue face of the Blade. When the mini-toolbar appears, click the third button on the right, labeled with the tooltip Create Sketch. Now we are in the sketch environment. Take the project of the model by using Project Cut Edges tool. Select all the sketches in the design window and convert them into construction geometry. Create tooth profile with the help of line tool. Now the sketch is complete. Finish the 2D sketch. Select any line of the enclosed profile, the mini-toolbar appears in the graphics window. Click the Create Extrude icon. It will automatically select the tooth profile. Extrude dialog box is visible in the design window. In the Extents field, select ‘All’ option from the drop down list. It will automatically select the ‘Cut’ operation. Click OK to create the feature. Click the ‘Rectangular Pattern’ icon on the Pattern panel of 3D Model tab. Rectangular Pattern dialogue box is visible in the graphics window. Features button is active by default. Select Extrusion3 from the browser bar. Right click in the graphics window and choose Continue. Select horizontal edge of the blade parallel to X Axis to define the direction of pattern. Choose the Flip button to reverse the direction. Set the column count to 192. Set the column spacing to 0.0625 inch. Now the preview of pattern is visible. Click OK to execute the Rectangular Pattern Feature. Right click the Rectangular Pattern2 in the browser bar, and then select Show Dimensions.
Application of ‘Text’ tool and ‘Emboss’ tool-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 192 Application of ‘Text’ tool and ‘Emboss’ tool-Autodesk Inventor 2013 (with caption and audio narration) In this exercise a pre constructed part file ‘Anvil’ is used. Click the following link to get the model file: – http://bit.ly/2nJyMTG Transcription of Video Open the Anvil (.ipt) file. At present a pre constructed part file of ‘Anvil’ is visible in the isometric view. Create a new sketch on the blue face of the Anvil with the help of ‘Create 2D Sketch’ tool. Take the project of the model by using ‘Project Cut Edges’ tool. Select the projected model edges in the design window and convert them into construction geometry. Start the ‘Text’ tool from the Draw panel of the Sketch tab. In the graphics window, click to place the insertion point for the text box and drag to define the area of the text box. Format Text dialogue box is visible in the graphics window. In the ‘Format Text’ dialogue box, enter the text ANVIL in the specified area. Select text and choose Center Justification and Middle Justification in the ‘Style’ option. Enter the value 0.8 in the ‘Size’ field. Change the text colour to Red. In the ‘Font’ field, select ‘Calibri’ font from the drop down list. Click OK to place the Text. Right click in the graphics window and click OK to finish the command. Apply Vertical constraint and Coincident constraint on the text to position it properly. Finish the 2D sketch. Activate the ‘Emboss’ tool from the Create panel of the 3D Model tab. Emboss dialogue box is visible in the design window. The profile selection is activated by default. Select text as profile. In the ‘Depth’ field enter the value 0.25 inch. Change the direction of the feature by clicking the flip direction button. Click OK to execute the Emboss feature. Select the Emboss feature in the browser bar and activate the ‘Adjust’ tool from the ‘Quick Access Tool Bar’. Adjust the appearance tinting of the feature and click OK to apply.
Can (Autodesk Inventor 2013)
Serial No. 185 Can (Autodesk Inventor 2013) Click the following link to get the model file: – http://bit.ly/2mPuGJP
Application of ‘Extrude’ tool (Join operation) Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 191 Application of ‘Extrude’ tool (Join operation) Autodesk Inventor 2013 (with caption and audio narration) Click the following link to get the model file: – http://bit.ly/2omKELY Transcription of Video Open the Part1 file. A pre constructed sketch1 is visible in the design window. Double click the Sketch1 in the browser bar. Take the Offset of sketch, of the value 1/4 inch inside the enclosed profile. Activate the extrude command from the marking menu. Extrude dialogue box is visible in the design window. The Profile selection button is active by default. Select the profile enclosed by the yellow sketch and enter the distance value 3/8 inch. Click OK to apply the extrude feature. Open the visibility of Sketch1. Activate the Extrude command once again from the Create panel. Select the profile enclosed by the yellow lines and extrude it 1 inch in upward direction.
Creating a Realistic Thread (Autodesk Inventor 2013)
Video Tutorial with caption and audio narration The Screw file displayed in the video is taken from our model ‘Knob of Switch’. First of all get the model files required to complete this tutorial by visiting the following link:- http://bit.ly/32leYVx Transcription of Video 1. Open the part file of Screw.2. Select the ‘Thread’ tool in the Modify panel of 3D Model tab.3. ‘Face’ selection button is automatically activated in the Thread dialogue box.4. Select blue cylindrical face of the Screw.5. Click the Specification tab, here it has automatically detected features/values like ‘Thread Type’, ‘Size’, ‘Designation’, ‘Class’ and ‘Right Hand thread’.6. If anyone wants to change the properties/features, it can be edited very easily.7. Click OK to apply the thread feature.8. Select the ‘Thread Modeler’ tool in the Thread Modeler panel of Tools tab.9. Select Thread feature in the Browser Bar.10. The Thread Modeler tool has automatically detected the pitch of the thread in the Thread Modeler Control dialogue box.11. Click OK to apply realistic thread on the screw.………………………………………………………………………………………………………………………………….. Visit Autodesk exchange Apps site on the following link to get the ‘Thread Modeler Tool’ which is an external application utilized with the software :- http://apps.exchange.autodesk.com/INVNTOR/de/Detail/Index?id=appstore.exchange.autodesk.com%3Athreadmodeler_windows32and64%3Aen
Knob of Switch-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 184 Knob of Switch-Autodesk Inventor 2013 (with caption and audio narration) Click the following link to get the model file: – http://bit.ly/2nI2Q2o Transcription of Video Modelling a ‘Knob of Switch’ (Autodesk Inventor 2013) Open a New Standard (in).ipt file. Create a new 2D sketch on the XY Plane. Draw a circle of 1 ¾ inch diameter, coincident with the auto projected part origin. Click Finish 2D Sketch command from the marking menu to exit the sketching mode. Activate the ‘Extrude’ Command. It will automatically select the circle as profile. Enter the extrusion value ¼ inches and click OK. Change the colour of the model to ‘Flaked Reflective – Beige’. Save the file with the name ‘Knob of Switch’. Change the view of the model by using View Cube. Set the view as Home View by clicking the toggle next to View Cube. Start a new sketch on the top face of the model. Take the project of circular edge and Y Axis. Convert this vertical line and circle into construction geometry. Draw an arc over the projected edge of the model with the help of Centre Point Arc tool. Apply a Coincident Constraint between mid-point of Arc and projected Y Axis line. Give a linear dimension 1/4 inch between both the end points of the arc. In the same way, draw another centre point arc as displayed. Apply a Coincident Constraint between mid-point of arc and Y Axis. Give a linear dimension 1/2 inch between both the end points of the arc. Finish the sketch. Create a new Work Axis on the one end of the arc, parallel to Z Axis of the model. Create a new Work Point at the intersection of Work Axis 1 and bottom circular edge of the model. Create a new work plane by using Three Point work plane tool. Close the visibility of Work Point1 and Work Plane1. Start a new sketch on this work plane. Take the project of the model by using Projected Cut Edges tool. Draw two vertical lines on both the end points of the top projected edge of the model. And apply dimension 1 inch on these two lines. Close the profile by using line tool. Convert the sketches into construction geometry which are presently not in use. Exit from the sketching environment. Create another Work Axis on the second end point of the arc, parallel to Z Axis of the model. Create another Work Point at the intersection of Work Axis 2 and bottom circular edge of the model. Create a new work plane by using Three Points work plane tool. Start a new sketch on this work plane. Take the project of the model by using Projected Cut Edges tool. Draw two vertical lines on both the end points of the top edge of the model. And apply dimension 1 inch on these two lines. Close the profile by using line tool. Convert the sketches into construction geometry which are presently not in use. Exit from the sketching environment. Create another 3 Point work plane on the top end points of these lines. Create a new sketch on this work plane. Take the project of both arcs on this work plane. Finish the sketch. Start the Loft tool. First select both the closed sketch profiles in the design window. Then select four arcs as rails. Click OK to create the Loft feature. Create a new sketch on the top face of the model. Take the project of top face of model by using Project Geometry tool. Create a new sketch profile with the help of Offset tool. Affix offset distance 1/32 inch between the lines. Take the offset of upper and lower segment of arc. Affix offset distance 5/16 inch between the arcs. Snap the end points of arcs with the adjacent lines by using coincident constraint tool. Erase the extra lines and arcs with the help of Trim tool. Finish the 2D sketch. Cut the enclosed area (defined by Sketch6) 1/32 inch towards downward direction by using Extrude Command. Pick up the Fillet tool. Select this circular edge of the top face, enter the value 1/4 inch in the Radius input box and click OK. Apply another fillet of value 1/8 inch on the opposite side of the previous circular edge. Rotate the model by using View Cube. Create a new sketch on the bottom face of the model. Take the project of bottom face of the model with the help of Project Geometry tool. Create a new circle with the help of Offset tool. Affix offset distance 1/8 inch between these two circles. Finish the sketch. Cut the enclosed area (defined by Sketch7) 3/16 inch towards downward direction by using Extrude Command. Create a new sketch on the inner circular face of the model. Draw a circle of diameter 5/8 inch and extrude this circle to 1/8 inch. Create a new sketch on the YZ Plane of Knob-Switch. Right click in the design window and select Slice Graphics command. Take the project of Z Axis of the model and outer vertical edge. Select both the vertical lines and change their colour to white. Draw a horizontal line. Place dimension ¼ inch between bottom edge of the model and horizontal line. Select both the vertical lines and convert them into construction geometry. Draw a vertical line of 1/32 inch length over the projected Z Axis of the model. Draw an arc coincident with these two points with the help Three Point Arc tool. Create another horizontal line and apply a tangent constraint between arc and this line. Activate the Revolve tool from the right click context menu. It will automatically select the sketch profile. Click on this line to specify the axis of revolution and click on green checkmark. A smooth oval face is created. Rotate the model on the back side. Create a new sketch on the blue circular face. Draw a circle of diameter 5/16 inch, coincident
Application of Combine Tool (Join operation) Autodesk Inventor 2013
Video Tutorial with caption and audio narration In this video tutorial two pre-constructed parts have been utilized to show Boolean operation in a part file, by using ‘Combine’ tool that is available in the Modify panel of 3D Model tab. First of all get the model files required to complete this tutorial by visiting the following link:- http://bit.ly/2oQSwpv Transcription of Video 1. We have two files one is Cylinder and the other is Example Insert.2. Open the Cylinder file.3. Activate the Derived Component tool.4. Select the Example Insert file and open it.5. Click OK to place the Example Insert in the design window.6. Re-orient the model in the design window by using View Cube.7. Change the Visual Style to Shaded with Hidden Edges to see the Example Insert clearly.8. Two separate solid bodies are visible clearly in the Browser Bar.9. Close the visibility of Cylinder.10. Activate the Measure Tool from the Marking menu.11. Take the measurement of this edge.12. Measurement of the edge is 0.5 inch.13. Open the visibility of Cylinder.14. Start the Move Bodies tool.15. And then select Example Insert.16. Enter value 0 inch in the X Offset input box.17. To move the Example Insert in Z direction.18. Enter value (-0.5) inch in the Z Offset input box and click OK.19. Activate the Combine tool.20. Join option is selected by default.21. Select both the solid bodies in the design window.22. Click OK to close the dialog box.23. Now checkout the Browser Bar, only one solid body exists.
Application of Combine Tool (Cut operation) Autodesk Inventor 2013
Video Tutorial with caption and audio narration In this video tutorial two pre-constructed parts have been utilized to show Boolean operation in a part file, by using ‘Combine’ tool that is available in the Modify panel of 3D Model tab. First of all get the model files required to complete this tutorial by visiting the following link:- http://bit.ly/2ClzJpi Transcription of Video 1. We have two files one is Cylinder and the other is Example Insert.2. Open the Cylinder file.3. Activate the Derived Component tool.4. Select the Example Insert file and open it.5. Click OK to place the Example Insert in the design window.6. Re-orient the model in the design window by using View Cube.7. Two separate solid bodies are visible clearly in the Browser Bar.8. Activate the Combine tool.9. First select Cylinder as a base body. 10. And then select Example Insert as a tool body.11. Join option is selected by default.12. Select Cut option to remove the material from Cylinder Part.13. Click OK to close the dialog box.
