Application of ‘Loft’ tool Ex.2–Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 200 Application of ‘Loft’ tool Ex.2–Autodesk Inventor 2013 (with caption and audio narration) In this exercise, we are using a partially constructed model of ‘Mug-Plastic’. We will create a Handle on the curve surface of the model, for this we will add some 2D sketches, work planes and Loft feature. Click the following link to get the model file: – http://bit.ly/2nNFfgo Transcription of Video Open ‘Mug-Plastic’ part file. Create a new work plane 0.25 inch below from the top face of the model. Create a new sketch for upper portion of handle on the newly created work plane. Right click in the graphics window and select Slice Graphics command. Take the project of the model by using Project Cut Edges tool. And with the help of Project Geometry tool, take the project of XY Plane. Select all the sketches in the design window and convert them into construction geometry. Now proceed further and draw a sketch with the given dimensions. Exit from the sketching environment. Close the visibility of Work Plane8 from the Browser Bar. Create another work plane named 9, 3 inch below from the top face of the model. Create a new sketch for lower portion of handle on Work Plane9. Close the visibility of work plane and activate the Slice Graphics command. Draw the sketch with the given dimensions. Now the sketch is complete. Finish the sketch. Activate the ‘Loft’ tool. Select the upper and lower sketch profiles in the graphics window. Preview of Loft is visible. Click OK to execute the loft feature. Open the visibility of Sketch17 from the Browser Bar. Create a new sketch on Work Plane8. Take the project of these two lines and arc. Draw a centre point arc between point1 and point2 (indicated by blue colour). Close the visibility of Sketch17 from the browser bar. Revert these two construction lines into regular lines. Exit from the sketching environment. Create a new work plane named 10, 0.0625 inch below from the top face of the handle. Auto-Resize the work plane. Create a new sketch on work plane 10. Activate the Slice Graphics command. Close the visibility of Work Plane10. Take the project of the model by using Project Cut Edges tool. And with the help of Project Geometry tool, take the project of XY plane. Convert all the sketches in the graphics window into the construction geometry. Draw the sketches as displayed. Finish the sketch. Activate the Loft tool once again. Select the upper and lower enclosed profiles, created over the handle. And click OK to execute the loft feature. Now most of the portion of the handle is complete. Save the part file.
Double Sided Half V-Groove Weld Joint-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 28 Double Sided Half V-Groove Weld Joint-Autodesk Inventor 2013 (with caption and audio narration) Click the following link to get the model file: –http://bit.ly/2n4rHgu Transcription of Video Create a New Standard (in).ipt file. Draw a new sketch on XY Plane. Draw a Rectangle of sides 1 inch and 1/8 inch with the help of ‘Three point Centre Rectangle’ tool. The center point of the rectangle should lie on the auto projected part origin. Take the project of X Axis of part file by using Project Geometry tool. Select all the sketches in the graphics window and convert them into construction geometry. Add two more lines in the sketch and apply Symmetric constraint between them. And apply 45 degree dimension between these two lines. Close the profile by using line tool. Finish the 2D sketch. Select any one of the line of enclosed profile, a mini-toolbar will appear in the graphics window. Click the ‘Create Extrude’ icon. Extrude dialogue box is visible in the graphics window. In the Extents field, select ‘Symmetric’ option. Fill the value 2inch in the distance input box. Click OK to create the extrude feature. Change the model colour to ‘Flaked Reflective – Beige’. Save the part file with its default name (Part1). Close the part file. Create a New Standard (in).iam file. Place two instances of ‘Part1’ in the assembly with the help of ‘Place Component’ tool. Save the Assembly with the name ‘Double Sided Half V-Groove Weld Joint’. Click the ‘Rotate’ icon on the Position panel of Assemble tab. Select Part1:2 in the design window and rotate the part as displayed. Right click in the graphics window and click OK to close the tool. Activate the Constraint command from the marking menu. Place Constraint dialogue box is visible in the graphics window. By default ‘Solution Type’ is set to Mate, change it to Flush. Select the top face of both parts to apply a flush mate. Apply a Flush mate once again but this time select front face of both parts. Apply a Mate constraint between side edges of both parts. Now our assembly is fully constrained. There is no degree of freedom. To apply a weld between these parts convert the assembly into weldment , click the ‘Convert to Weldment’ icon, located on the Convert panel of Assemble tab. Click Yes button, when prompted that you will not be able to revert this data to a basic assembly. Convert to Weldment dialogue box is visible in the graphics window. Leave the default settings click and OK to close the dialogue box. Double-click the ‘Welds’ group in the browser to activate the weldment tools. Activate the ‘Groove Weld’ tool, located on the Weld panel of Weld tab. Groove Weld dialogue box is visible in the graphics window. Select the Full Face Weld check box in the Face Set 1 and Face Set 2 under the Bead box field. Click the Face Set 1 button. Select this face of the Part. Click the Face Set 2 button. Select this face of adjacent part. Click OK to create a groove weld between the both parts. In the same manner apply another groove weld over the rear side of the model. Save the Assembly.
Modeling a Link of a Chain (Pro E Wildfire)
The following video will display the modelling of Link of a Chain. This is a part modelling video, so viewers will see the application of many part modelling tools of Pro E Wildfire 5.0 (Extrude, Hole, Mirror, Round etc.) as well as 2D sketch tools. To get finished files displayed in the video visit following link—– http://bit.ly/2nrq6kU I have used this ‘Link’ in the creation of Chain Animation in the past, whose video ‘Chain-Inventor Studio Autodesk Inventor is available on the following link: — http://nisheeth-inventortalks.blogspot.com/2011/05/chain-inventor-studio-video-tutorial.html
Application of ‘Contour Flange’ & ‘Contour Roll’ tool-Autodesk Inventor 2013 (with caption and audio)
Serial No. 199 Application of ‘Contour Flange’ & ‘Contour Roll’ tool-Autodesk Inventor 2013 (with caption and audio) Transcription of Video This is the model of Square Bend Tube that is created by us earlier. A full-fledged video related to this can be found on our You Tube Channel. Here from the Browser Bar you can check the history of its modelling. Contour Flange and Contour Roll were used to create this model. In this video we will describe about the aforesaid features and show how they work. Contour Flange Feature Contour Flange tool is available on Create panel of Sheet Metal Tab. Contour Flange is used when you have created an open sketch profile with the help of lines, arcs, splines or elliptical arcs etc. and you want to create a flange on basis of it. When you want to create a flange on basis of a sketch profile created with the help of lines, arcs, splines or elliptical arcs etc. then Contour Flange is used. The most important requirement for this tool is an open sketch profile; you cannot use this tool with a closed sketch profile. Contour Flange applied in the modelling of Square Bend Tube (First instance) This is the open sketch profile that is used for flange creation. After activating the Contour Flange Tool, select the sketch profile that is visible in the graphics window. Distance is automatically set as Width Extents Type. Distance value 200 mm is filled already. From here you can flip the extent direction. Click OK to create the Contour Flange feature. Contour Flange applied in the modelling of Square Bend Tube (Second instance) This time the visible projected edge of the model will be used to create sheet metal flange. Activate the tool and select the visible sketch having the projected edges of the model. Expand the more button to find additional option of Contour Flange dialogue box. Set the Width Extents Type to Distance. Fill the distance value 200 mm. Click OK to create the Contour Flange feature. Contour Roll Feature Contour Roll Feature is used to revolve an open sketch profile around an axis to develop a sheet metal flange. This tool is available on the Create panel of Sheet Metal Tab. Contour Roll applied in the modelling of Square Bend Tube (First instance) This is the open sketch profile consisting projected model edges and an axis. After activating the Contour Roll Tool, select the sketch profile visible in the graphics window. Now Axis selection is active so select the axis for revolution. Fill 30 degree in Rolled Angle input box. Click OK to close the Contour Roll dialogue box. Contour Roll applied in the modelling of Square Bend Tube (Second instance) This time the visible projected edge of the model will be used to create sheet metal flange. Activate the Contour Roll Tool and follow the same procedure, as applied earlier to create the Contour Roll feature. The final result is visible in the design window.
Application of ‘Sweep’ tool and ‘Circular Pattern’ tool-Autodesk Inventor 2013 (with caption and audio)
Serial No. 198 Application of ‘Sweep’ tool and ‘Circular Pattern’ tool-Autodesk Inventor 2013 (with caption and audio) In this exercise we will create a new part named ‘Blade-base’, related to our previously created full-fledged model ‘Mixer (Cabinet)’. In this part file we will utilize following feature/tools: – 2D Sketches, work planes, extrude, fillet, sweep and circular pattern. Click the following link to get the model file: – http://bit.ly/2nMCMms Transcription of Video Create a New Standard (in).ipt file. Create a new sketch on the XY Plane with the aid of ‘Create 2D Sketch’ tool. Draw the sketch diagram of part ‘Blade-base’ with the help of line tool. Pick up the Offset tool and select all lines in the graphics window. Enter the offset distance 1/16 inch between these two lines. Close the sketch profile by adding lines where the gap exists. Now the sketch is complete. Finish the 2D sketch. Select any one of the line of enclosed profile, the mini-toolbar will appear in the graphics window. Click the ‘Create Extrude’ icon. It will automatically select the enclosed profile. Extrude dialogue box is visible in the graphics window. In the Extents field, select ‘Symmetric’ option. Enter the distance value 3/8 inch. Click OK to create the extrude feature. Change the model colour to ‘Steel’. Save the file with the name ‘Blade-base’. Activate the Fillet tool from the Modify panel of 3D Model tab. Fillet dialogue box is visible in the graphics window. Select four bend edges of the model. Set the value to 1/16 inch in ‘Radius’ field. Click OK to create the fillet feature. Now make some changes in the settings of the software. Go to the Options panel of Tools tab and click Application Options icon. Application Options dialogue box is visible in the graphics window. General tab is active by default. Switch to Sketch tab. Click on the Standard Toggle box of ‘Autoproject edges for sketch creation and edit’ option. Apply and close the dialogue box. Create a new sketch on the blue face of the model, it will be used as a profile for the sweep. Select the projected model edges in the graphics window and convert them into construction geometry. Draw a line from Point1 of length 1/8 inch, parallel to Z direction of prevailing 3D indicator in the graphics window. Draw another line from the same Point1 of length 3/64 inch, parallel to Y direction. Close the profile by adding a new line. Finish the 2D Sketch. On the Ribbon click ‘Plane’ icon on the Work Features panel of 3D Model tab. Click on Point2 and select corresponding edge of the model (indicated by red colour). Work Plane has been created, perpendicular to this edge. Create a new sketch on this Work Plane to create a path for sweep. Right click in the graphics window and choose ‘Slice Graphics’ option. Take the project of the model by using ‘Project Cut Edges’ tool. Convert the entire projected model edges into construction geometry except yellow coloured line and arc. Add a new line starting from Point3 of length 0.75833 inch over the projected model edge indicated by yellow colour. Finish the 2D Sketch. Activate the ‘Sweep’ tool from Create panel of 3D Model tab. Sweep dialogue box is visible in the graphics window. Since there is only one closed profile, the profile drawn on Sketch2 is selected automatically. The Path selection button is active in the Sweep dialogue box. Select the sketch profile drawn on Sketch3 as sweep path in the graphics window. Select ‘Cut’ option to remove the material. Click OK to execute the Sweep feature. On the Ribbon click ‘Circular Pattern’ icon on the Pattern panel of 3D Model tab. Circular Pattern dialogue box is visible in the graphics window. In the Circular Pattern dialogue box, ‘Features’ selection button is activated by default. Select the ‘Sweep1’ in the Browser Bar as feature to pattern. Right click in the graphics window and choose Continue from the context menu. Select the Y Axis in the Browser Bar to define axis of revolution. Set the pattern count value 2 in the ‘Placement’ field. Leave the pattern angle 360 degree unchanged which is set by default. Click OK to execute the Circular Pattern feature. Create a new sketch on the blue face of ‘Blade-base’. Draw a square of length ¾ inch with the aid of ‘Three Point Centre Rectangle’ tool, coincident with autoprojected part origin. Activate the ‘Three Point Centre Rectangle’ from the Draw panel of Sketch tab. Click on Point4 to set the center point of the rectangle. Right click in the graphics window and click OK to finish the rectangle command. Exit the sketching environment. Activate the Extrude command from the marking menu. And select the square. In the Extents field, select ‘To’ option from the drop down list. Select back face of the model and choose Join option. Click OK to create Extrude feature. Create a new sketch once again on the blue face of model. Draw another square of length 3/16 inch. Use this square to remove material from the model by using Extrude tool.
Application of ‘Circular Pattern’ tool-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 197 Application of ‘Circular Pattern’ tool-Autodesk Inventor 2013 (with caption and audio narration) Transcription of Video This is the model of Twist Drill that is created by us earlier. A full-fledged video related to this can be found on our You Tube Channel. Here from the Browser Bar you can check the history of its modelling. A lot of 2D sketches, Extrude, Coil features, Work features and Circular Pattern were utilized to create this model. In this video we will describe about the Circular Pattern Tool that was used three times in its modelling. Watch the video to understand how the tool works. Circular Pattern tool duplicates one or more features and arrange the resulting occurrences by a specific count and spacing in a circular path. This tool is available on Pattern Panel of Model Tab. First Circular Pattern Applied in the modeling of Twist Drill After activating the Circular Pattern tool the Coil1 and Extrude2 are being selected as feature for the duplication. Z axis of the model has been selected as axis of revolution. The number of occurrences in the pattern is 2. Degree of rotation is 180. After clicking the ok button the result is in front of you. A duplicate feature is created easily. Watch the past and current position of the model by suppressing and un-supressing the feature. Second Circular Pattern Applied in the modeling of Twist Drill. This time Extrude4 is selected as feature and the Rotation of Axis is same that is the Z axis of the model. The Occurrence count will be 2 and the Occurrence angle180 degree. After clicking the ok button the duplicate feature is created. Third Circular Pattern Applied in the modeling of Twist Drill. This time two Coil features are selected for the duplication. All the other specifications of the Circular pattern will be the same as previous ones. The final result is visible in the design window.
Application of ‘Sweep’ tool and ‘Shell’ tool-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 196 Application of ‘Sweep’ tool and ‘Shell’ tool-Autodesk Inventor 2013 (with caption and audio narration) In this exercise we will create a new part, related to our previously created full-fledged model ‘Elbow’. In this part file we will create some 2D Sketches, work planes, sweep & shell features. Click the following link to get the model file: – http://bit.ly/2nPe9Wf Transcription of Video Create a New Standard (in).ipt file. Create a 2D Sketch on the XY Plane. Draw a line of length 1.1875 inch, coincident with the auto projected part origin and parallel to X axis. Right click in the graphics window and select ‘Create Line’ tool. Click the green point in the graphics window as start point of the line. And enter the value 1.1875 inch. Right click in the graphics window and click OK to finish the command. Create another line of length 1.1875 inch, parallel to Y axis and coincident with the origin. Select these two lines and change the colour to White. On the Ribbon click ‘Fillet’ icon on the Draw panel of Sketch tab. 2D Fillet dialogue box is visible in the graphics window. Enter the value 0.625 inch in the 2D fillet dialogue box. And select these two lines in the graphics window to apply the fillet. Right click in the graphics window and click OK to exit the command. Finish the 2D Sketch. On the Ribbon click ‘Plane’ icon on the Work Features panel of 3D Model tab. Click one of the end points of the line and select this line in the graphics window. Work Plane has been created, perpendicular to this line. Create a new sketch on this Work Plane. Draw a Circle of diameter 1 inch on the end point of the line. Finish the 2D Sketch. Activate the ‘Sweep’ tool from Create panel of 3D Model tab. Sweep dialog box is visible in the graphics window. Since there is only single closed profile, the profile drawn on sketch 2 is selected automatically. The path selection button is active in the Sweep dialogue box. Select the ‘Sketch1’ in the graphics window as sweep path. Click OK to execute the Sweep feature. Change the model colour to ‘Flaked Reflective – Beige’. Save the Part file with the name ‘Elbow’. On the Ribbon click ‘Shell’ tool icon on the Modify panel of 3D Model tab. Shell dialog box is visible in the graphics window. ‘Remove Faces’ selection button is activated by default. Select both blue faces of the Elbow. Enter the value 0.125 inch in the ‘Thickness’ field. Click OK to apply the Shell feature.
Application of ‘Loft’ tool Ex.1-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 195 Application of ‘Loft’ tool Ex.1-Autodesk Inventor 2013 (with caption and audio narration) In this exercise, we are using a partially constructed assembly of ‘Grating for Gas Oven’. We will add some 2D sketches, work planes and a loft feature to proceed towards its completion. Click the following link to get the model file: – http://bit.ly/2otrMLl Transcription of Video Open the ‘Grating for Gas Oven’ (.iam) file. Here a pre constructed ‘Part1’ is visible in this Assembly. Activate the ‘Create Component’ tool to create a new part in the Assembly. Select the XY Plane of the assembly as a base plane for the new component. Create a new sketch on the XY Plane of the ‘Part2’. Take the project of Part1 by using ‘Project Cut Edges’ tool. Select the projected model edges in the graphics window and convert them into construction geometry. On the Ribbon, click ‘Finish Sketch’ icon. Now we will create a new work plane, parallel to YZ Plane of Part2 with the aid of ‘Offset from Plane’ tool. Activate the ‘Offset from Plane’ tool from the Work Features panel of 3D Model tab. Select YZ Plane of ‘Part 2’ from the Browser Bar. Mini toolbar appears in the graphics window. Drag the manipulator arrow button in the graphics window. Enter the offset distance value (-1.875) inch. Click OK to create a new work plane. Create a new sketch on this work plane. Take the project of bottom edge of the Part1 and Y Axis of Part2. Convert both the projected edges into construction geometry. Draw a rectangle of value 0.25 inch X 0.349 inch with the help of ‘Three Point Center Rectangle’ tool. Apply a dimension of 0.2991 inch between center point of rectangle and projected edge of Part1. Finish the 2D Sketch. Create a new work plane parallel to Work Plane1 at an offset distance of 3.25 inch. Close the visibility of Work Plane1. Create a new sketch on Work Plane2. Take the project of top line of previously drawn rectangle. Close the visibility of Sketch1 and Sketch2 from the Browser Bar to clear the screen. Take the project of Y Axis of Part2. Create a new line of 0.4040 inch with the aid of Offset tool. Apply a Coincident Constraint between midpoint of newly created line and projected Y Axis line. Apply 0.59860 inch dimension between these lines. Add two more lines to close the profile. Finish the 2D Sketch. Open the visibility of Sketch2 from the Browser Bar. Activate the ‘Loft’ tool from Create panel of 3D Model tab. Loft dialogue box is visible in the graphics window. On the ‘Curves’ tab, specify the sections to loft. Click under the ‘Sections’ heading and the select both the sketch profiles in the graphics window. Click OK to execute the Loft feature. Close the visibility of Sketch2 and Work Plane2 from the Browser Bar. Change the colour of model to Steel. Return back to the Assembly environment.
About Nivesh and Nisheeth
We are two brothers, Nisheeth Srivastava (date of birth 02-05-1980) and Nivesh Srivastava (date of birth 27-07-1985). We reside in India. We started learning computer software by ourselves at home. We haven’t joined any institute to learn computer application software up till now. We simply bought a computer, afterwards, we also bought a Notebook and arrange some software according to our choice and started learning with our own sincere efforts. By the mercy of God, we began to follow some fundamental aspects of the application in computer software, which developed an interest to us in the computer world. First, we learned ‘Microsoft Word’, ‘CorelDraw’, ‘Adobe Pagemaker’ & ‘Adobe Photoshop’ up to a moderate level along with ‘English language’ & ‘Hindi language’ computer typing. After this, we started learning ‘AutoCad’ software. This created an interest to work in a 3-D environment and began to look forward to more advanced software. At present, our favourite software is ‘Autodesk Inventor Professional’, we are practising more and more and trying to make the more precise drawing with the aid of this 3-D Parametric software. We have created One hundred thirty-one Video Tutorials ‘3-D Parametric Solid Model Drawings — 2010 & 2012’, which are already uploaded on our ‘YouTube’ Channel and their ‘Autodesk Inventor Drawing Files’ are uploaded on ‘Mediafire’ hosting site. http://www.youtube.com/user/niveshandnisheeth http://www.youtube.com/user/NISHEETHSORJM We have also created a Blog— http://niveshandnisheeth.blogspot.com We want to gain practical training as a ‘Drafter’ in designing of 3-D parametric solid model drawing in the real world, in any factory/company that is using Autodesk Inventor software. We do not demand any stipend (within our native country) during this period from the company. Also, we do not insist to give any commitment of a job in that concern after the completion of our training. If anyone provides us with a chance for training, we assure that we will follow rules and regulation of the company with most sincerely an honestly. We request to help us in this regard, by providing a platform to start our career for a job in Autodesk Inventor. E-mail:— niveshandnisheeth@gmail.com Address:- 638, Malviya Nagar Allahabad 211 003, State: – U.P. (India) Date: — March 30, 2013
