Application of Extrude Feature-Autodesk Inventor 2013 (with caption and audio narration)
Serial No.150 Application of Extrude Feature-Autodesk Inventor 2013 (with caption and audio narration) In this Video, we have focused mainly on Extrude Feature and its application to make ‘Part7’ of previously created model ‘LED Lamp’. Click the following link to get the drawing sheet of the model: – http://bit.ly/2nL6ybg Transcription of Video Application of Extrude Feature In this Video we have focused mainly on Extrude Feature and its application to make ‘Part7’ of previously created model ‘LED Lamp’. At present you are watching a work piece in the design window. Its name is ‘Part7’ which is taken from our previously created model ‘LED Lamp’. We want to develop this work piece like this. In the following steps we will start adding some more features. We will start our work by creating a new Work Plane that would be tangent to surface of this work piece. Draw a new sketch on this Work Plane which is defined as sketch6 in the Browser. Take the project of XY Plane with the help of ‘Project Geometry’ Tool. Start a Rectangle Tool Command and fill the dimension. Apply Coincident Constraint between the rectangle and vertical line. Now the rectangle is centred over the vertical line. Now take the project of this edge and convert it to construction mode. Now apply Collinear Constraint between horizontal line of the rectangle and the construction line. Now draw an arc over the top edge of this rectangle, next convert this line into the construction geometry. Take another project of this edge. Draw a line over this edge and centre align it with the vertical line. Draw an arc again. Apply the dimension as displayed. Create a triangular shape drawing with given dimensions. Now this sketch is complete. Select Work Plane2, right click and turn off its visibility. Extrude sketch6-a and select the ‘Cut’ option and click OK. Fill the dimension 0.12475 inch to remove the unwanted material. In the browser click the small plus icon beside the Extrusion5 and select Sketch6, right click and select share sketch, you will see that Sketch6 is visible. (By using ‘Share Sketch’ option we can reuse a previously drawn sketch feature). Now activate the ‘Extrude’ feature once again and select Sketch6-b and cut this section. Create a new sketch on this face. Extrude the surface enclosed by inner circle and cut it by 1/8 inch. Go to ‘Circular Pattern’ Tool, select Extrusion5 and Extrusion6 from the Browser Bar and define the axis of revolution by selecting the circular surface of this face and fill eight occurrences in the ‘Placement’ option and click OK. Create a circular flat ring of width 1/32 inch and extrude this sketch to 1/4 inch. Create one other circular strip of width 1/32 inch outside the previously created inner ring and extrude this sketch to 1/8 inch. In the next step we go to ‘Shell’ Tool and select the desired face and fill thickness 1/32 inch and click OK. Finally we found the desired shape of Part7.
Creating wires in Mesh of Table Fan-Autodesk Inventor 2013 (with caption and audio narration)
Serial No.149 Creating wires in Mesh of Table Fan-Autodesk Inventor 2013 (with caption and audio narration) …………………………………………………………….. This video will display how to create wires of the mesh of our previously created model ‘Mesh of Table Fan’. Click the following link to get the drawing sheet of the model: – http://bit.ly/2neUSNX Transcription of Video Creating wires in Mesh of Table Fan This video will display how to create wires of mesh of our previously created model ‘Mesh of Table Fan’. At present there are three components Part1, Part2 and Part3 in the Assembly. And we want to create 3 more new components Part4, Part5 and Part6 like this. We will start our work with creating a new component in the Assembly. At present the newly created component is not fully constrained in the Assembly, which can be confirmed by checking the ‘Degrees of Freedom’. To fully constrain it in the Assembly, we will apply Mate Constraint between Center Point of Part4 and Center Point of Assembly. Next, we will apply a Mate Constraint between Z Axis of Part4 and Z Axis of Assembly. And finally a Mate Constraint between XZ Plane of Assembly and XZ Plane of Part4. Now the Part is fully constrained, there are no Degrees of Freedom left. In this Assembly, a ‘Component Pattern’ feature was applied to replicate the Part3. We will ‘Suppress’ this feature and make visible only one instance of the Part3. By double clicking the Part4, we will now enter in the Part Modelling environment. Our first sketch will be drawn on the XZ Plane of Part4. First we will project the edges of the other components available in the Assembly, using the ‘Project Cut Edges’ Command. We will use these edges as a reference for creating new sketch. That is why we will apply a construction override on these projected edges. This will prevent them from being recognized as profiles by the 3D features. This offset length is equal to the radius of wire of mesh. Now we are applying constraints on our sketches to position it properly. This will also make our sketch Fully Constrained. We will create a Work Point on this newly created sketch and replicate it 22 times with the use of ‘Rectangular Pattern’ Tool. Select ‘Curve Length’ to place the Work Points along the path of the sketch. Now start a new sketch on the XZ Plane of Part4. Now project this Work Point on the sketch with the use of ‘Project Geometry’ Tool. Draw a circle on this point. Now we will develop our first wire of mesh with the help of ‘Revolve feature’. Change the colour of Part4 to ‘Steel’. Repeat the same steps to generate other wires of mesh. Clear the screen by activating the ‘Clean Screen’ Command. The fully developed Assembly will look like this.
Creating hole on a curve surface-Autodesk Inventor 2013 (with caption and audio narration)
Serial No.148 Creating hole on a curve surface-Autodesk Inventor 2013 (with caption and audio narration) ………………………………………………………………………. In this Video, we will show how to create holes on a Curved Surface using our Model ‘Strainer’. Click the following link to get the drawing sheet of the model: http://bit.ly/2o5IwIj Transcription of Video Creating hole on a curve surface In this Video we will show how to create holes on a Curved Surface using our Model ‘Strainer’. This is the model of ‘Strainer’ on which we want to create holes on it curved surface like this. First of all, we will enter in the part modelling environment by double clicking the Part1. We have already created Work Points on the curved surface of Strainer on the basis of a previously created sketch. These are all the Work Points, which you can see in the Browser Bar as well as in the design window. In the half section view, you can see it clearly that all the Work Points are landing on the curved face on the Strainer. This is the sketch on the basis of which all the Work Points were created earlier. A sketch of hole is required to create a hole on the Work Point. So first of all we will create a Work Plane on the Work Point that would be tangent to the curved surface of the Strainer. Take the project of Work Point and start the Circle Tool to create a circle of 0.03125 unit length. Finish the sketch. To create a hole on this sketch, we will use Extrude Command. Click Extrude from the Create Panel of 3D Model Tab. Click the circular profile. In the direction field, select ‘Symmetric’ option. Select ‘Cut’ option to remove the material from the curved surface of the Strainer and the hole is created. Turn off the visibility of the Work Plane. Now we will use the Circular Pattern Tool, that will replicate this extrude feature 80 times. First select the feature then the rotation axis. We will select the rotation axis as Y Axis from the Browser Bar. In the Placement field type 80. All the holes are now created. In the same way, we will create another hole on this Work Point. Same operations are being performed. This time we will activate the Extrude Command by just clicking the sketch, here you can see. The Extrude Command is visible there. In the second row, the circumference of the model has decreased, so we have to select less number of holes (i.e., 78 occurrences) in this Circular Pattern. In the same manner other holes can be created on the curved surface of the object easily, to get the desired result. Here is the finished Assembly of the Strainer you can see all the holes are here.
Creating a component in an assembly-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 147 Creating a component in an assembly-Autodesk Inventor 2013 (with caption and audio narration) This video will display how to create a component in the context of an Assembly. Creating a component in this way has many benefits. We can Project faces and edges of the Assembly in the new component. The faces of other components can be copied and placed on surfaces and many more things can be done. So watch the video to understand. Transcription of Video Creating a component in an Assembly This video will display how to create a component in the context of an Assembly. Creating a component in this way has many benefits. We can Project faces and edges of the Assembly in the new component. The faces of other components can be copied and placed as surfaces and many more things can be done. So watch the video to understand. We have an Assembly named ‘Mesh (Front)’ consisting two components ‘Part1’ and ‘Part2’. Now we want to create a new component named ‘Part3’ in this Assembly like this. The Vertical distance between Part1 and Part2 is 1.625 inch. We will start our work with creating a new component in this Assembly. The degree of freedom command shows that the newly created Part3 is not fully constrained with the Assembly. So we will apply a Mate Constraint between the Part3 and Assembly’s Z Axis. Next a Mate Constraint will be applied between XZ Planes of Assembly and Part3. In the following steps, we will create a loft feature in this component with the help of two sketches and a centre line rail. By double clicking the Part3 we will enter in the Part Modelling Environment. First of all we will get the edges of previously created components with the use of ‘Project Geometry Tool.’ These projected geometries are required only for reference. We are actually going to use these geometries in the developing the loft feature, that is why we will convert them in Construction Geometry. By applying Coincident Constraint we will properly position our geometry. Again unnecessary sketches will be converted into Construction Geometry. So we have created the required sketch now. Now we will create a New Work Plane parallel to YZ Plane of Part3 (7.625 inch away). Now we will create the remaining sketch on the XZ Plane of the Part3 that will be used for Centre line loft. From here we will change the colour of the Part to ‘Being Personal.’ In the next following steps we will develop the second loft feature in this Part. At present we are copying the outer face of the Part2 with the ‘Copy Object’ Tool. This will place a new surface component in this part. Now we will project this sketch on the previously created surface component with the help of ‘Project to 3D Sketch’ Tool. At present this 3D sketch is intact. We cannot use its one edge as a rail in the loft feature. So we will create a new 3D sketch and project its one edge in it with the use of ‘Include Geometry’ Tool. Repeat the same process to create the second Rail. In this way, we found our two separate rails required for the loft. Now we will create two 3D sketch profiles required for the loft. So everything is set. Start the ‘Loft’ Tool. Model edges can also be used as rails. So in this way we created our second loft feature in the Part3. We will now replicate this (Part3) 8 times at an angle of 45 degree by using ‘Pattern Component’ Tool, available at Component Panel of Assembly Tab. If you want to watch the development of other components, used in the ‘Mesh of Table Fan’ Assembly, watch our previous video named ‘Mesh of Table Fan’ (Autodesk Inventor 2010).
Rotate and Place components in an Assembly-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 146 Rotate and Place components in an Assembly-Autodesk Inventor 2013 (with caption and audio narration) In this Video we will describe about rotating and placing components in an Assembly. Transcription of Video Rotate and Place components in an Assembly In this Video we will describe about rotating and placing components in an Assembly. We have following components, which we want to place and constrain in an Assembly like this. So create a New Assembly File and start placing the components. The first component placed in an Assembly is always ‘Grounded’ and there is no need to constrain it. Now we are going to place the ‘Part8’ in the Assembly. To properly position the Part8 for Mate we will use ‘Rotate Component’ Command which is located in the Position Panel of Assemble Tab. After selecting the Part8, click anywhere outside the reticle to start the rotation. The component is positioned for the Mate now. Start the ‘Constrain’ Tool. Click this face and then this face. Now click Apply. The Rewind Tool is very useful to restore the most recent view or scroll through all of the save views. In the same way, other four Parts can be placed, positioned and constrained to get the desired result….. Now Assembly is fully constrained, there are no Degrees of Freedom that can be checked in this way…
Application of 3D sketch with loft feature-Autodesk Inventor 2012 (with caption and audio narration)
Serial No. 145 Application of 3D sketch with loft feature-Autodesk Inventor 2012 (with caption and audio narration) In this video, we will describe 3D sketch and its application in the creation of loft feature. Click the following link to get the drawing sheet of the model: http://bit.ly/2m51dLC Transcription of Video Application of 3D sketch with loft feature In this video we will describe about 3D sketch and its application in creation of loft feature. This is our sketch which is named Sketch5 in the browser. It is 2 inch up vertically from this point. This sketch is placed on the Work Plane5. Work Plane5 is 4.5 inch away from the Work Plane4. Now we want to connect Sketch5 to the cup of the Spoon like this. For this we will create two 3D sketches. Start a 3D sketch from the Sketch panel of the Model Tab. Create 3D line and close the sketch like this. Once again create another 3D sketch in the same manner. So the required two 3D sketches are in hand which we will use for developing the handle of Spoon. Now pick up the loft tool from the Create panel of the Model Tab and develop the handle of Spoon like this.
Application of browser bar in Autodesk Inventor (with caption and audio narration)
Serial No. 144 Application of browser bar in Autodesk Inventor (with caption and audio narration) In this video, we will tell you about the Browser Bar of Autodesk Inventor Software and its use. Autodesk Inventor is referred to as parametric solid modelling software. It maintains the history of how parts were constructed. The history will also show how they are related to one another in an Assembly. You can monitor this by observing the Browser Bar. Transcription of Video Application of Browser Bar in Autodesk Inventor In this video we will tell you about the Browser Bar of Autodesk Inventor Software and its use. Autodesk Inventor is referred to as parametric solid modelling software. It maintains the history of how parts were constructed. The history will also show how they are related to one another in an Assembly. You can monitor this by observing the Browser Bar. Browser in Part Modelling Environment How to observe history of parts. Currently we are opening the model of Anvil. This is the Browser Bar. From here you can check, what the designing process of this CAD Model was. Browser in Assembly Modelling Environment How to observe relation of Parts in the Assembly Currently we are opening the model of Shaving Razor. In the case of Assembly you can understand the history of modelling as well as relation of parts to one another by exploring the Mate Constraints.
Application of Split Tool-Autodesk Inventor 2012 (with caption and audio narration)
Serial No. 143 Application of Split Tool-Autodesk Inventor 2012 (with caption and audio narration) In this Video, we will describe ‘Split’ Tool and its application in cutting a segment from an intact face. Click the following link to get the drawing sheet of the model: http://bit.ly/2m51dLC Transcription of Video Application of Split tool In this Video we will describe about ‘Split’ Tool and its application in cutting a segment from an intact face. At present this face of the Spoon is intact. We need a segment of this face according to our design like this. To do so, first we will create a Work Plane on the top edge of the Spoon. Now we will create a line of 0.25 inch on this Work Plane. We will use the ends of this line to create new Work Planes later. These newly created Work Planes will be used as Splitting Tool. Now start the ‘Split’ Tool. Select ‘Split Face’ option in the Split tool dialog box. Select the Work Plane for the splitting tool. Use the Select face button for faces. Select the intact face of the Spoon and click Apply. Repeat the same process for next split. So this is the segment of face which was split. We can change the colour of this face to yellow. So that it can be recognized easily.
