Create a Wrench as an ‘iPart’ through-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 214 Create a Wrench as an ‘iPart’ through-Autodesk Inventor 2013 (with caption and audio narration) iParts are different from standard parts they are table driven part factories with a group of parts. The parts have the different parameter and different features that are controlled by table. The table is controlled by iPart Author or Spread Sheet. Click the following link to get the model file: – http://bit.ly/2nRnT2d Transcription of Video Activate the ‘Create iPart’ command. iPart Author dialogue box is visible in the graphics window. Notice that the columns for the named parameters had automatically displayed and iWrench-01 has been added to the current file to define the first family member’s part number. Discard all named parameters by clicking ‘Remove’ arrow button one by one and again place all these named parameters in desired sequence by using ‘Add’ arrow button. Click the Other tab button and fill the text in the ‘Name’ field. ‘Size’ column is automatically added in the table. Fill the value in size column. Right click the row of iWrench-01, and click Insert Row in the context menu. In the second row, change the value in each column for the new member. Click Verify button. Click OK to generate the iPart. Parameter Table has been added in the browser bar. Click the ‘+’ sign to expand the node. Right click the iWrench-02 node and choose ‘Activate’ option to change the size of the member. Activate the first member once again. Right-click the table icon and select ‘Edit via Spreadsheet’. The iPart table is opened in Microsoft Excel. Create another member in the excel file and enter the value in each column. More parameters can be added with the excel file. Save the spreadsheet and close it. Click Yes button to update the table. In the browser bar, the family members have been automatically added, it can also be seen from the Edit Table. Click Cancel button to close the dialogue box. Activate the each family member one by one and see the effect. Save the ‘iWrench’ file.
iWrench (Autodesk Inventor 2013)
Serial No. 213 iWrench (Autodesk Inventor 2013) This video tutorial features the designing process of a Wrench with the aid of Autodesk Inventor’s part modelling functionality.The highlight of the videos is the after creating the model with full parameters the iPart creation of the model is also displayed. Click the following link to get the model file: – http://bit.ly/2oIjPSX
Mounting Bracket || Creo Parametric 2.0 Sheet Metal Tutorial
In this tutorial I will create a Mounting Bracket by utilizing Sheet Metal capabilities of Creo Parametric 2.0 First of all base feature will be created using Planar Tool, afterward similar looking legs will be created using various tools like Extrude, Flange,Flat,Bend etc. Usage of Hole, Chamfer Round along with Flat Pattern Tool is also displayed. Transcription of Video Start a new Sheet Metal Part file from scratch with the default template and give it a name ‘Mounting Bracket’. 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. Activate the Circle Tool and draw the sketch with the dimensions as displayed. Convert this circle into construction geometry. Create a line in the sketch and duplicate it to the other side, using a centerline with the aid of Mirror Tool. Draw a new line and repeat the previous process for this line also. Create arcs between these lines by picking its centre and ends. Duplicate these arcs to other side using the Mirror Tool. Exit the sketch and activate Planar Tool. Fill the thickness of the sheet and execute the command after selecting the sketch. Change the colour of the model as per your wish. Create a sketch over Front Datum Plane. First specify new references, with which new sketch will be constrained and dimensioned. Draw the sketch using the Line Tool as displayed. Exit the sketch and activate the Extrude Tool. Select the sketch and activate Extrude both side of sketch plane equally option. Fill the extrusion depth. From the option tab activate add bends on sharp edges command, which would be equal to thickness of the sheet. Execute the command. Activate Flange Tool. Select an edge to attach the wall and then fill the length and angle of the wall. In the similar way add two more flanges. Activate the Flat Tool and first specify placement edge. Execute the command after defining the angle and length of the flat. Start a new sketch over top face of the model and draw a sketch similar to this one. First specify new references and use Line to draw the sketch at the defined position. Activate Bend Tool. First define the bend line and then fill the bend angle. Execute the command. Again repeat the same process to perform another bend operation. Hide the visibility of sketch3. Select the leg created with the extrude tool in the model tree and activate 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. Leave the default 90° Angle between the pattern members unchanged and execute the command. Save the file. Apply a Chamfer of 0.125 inch on the each of the legs. Activate the round tool and apply fillet of .06 inch on these edges of the model. Create a sketch on the top face of the model and draw a circle on this leg with the defined dimensions. Create a hole on the leg using this sketch and extrude tool. Open the visibility of Coordinate System and using its Y axis pattern the hole 4 times at an angle of 90°. Create a sketch on the top face of the model and create a point to define the position for the new hole. Activate the Hole Tool and select the point. Define the diameter of the hole and execute the command. Pattern this hole 6 times at an angle of 60°using Y axis of Coordinate System. The model is complete you can generate the Flat Pattern of the model. Note:– You may find holes inappropriate created with pattern tool on the leg, it is because the each leg is created with different feature and their flat pattern length is different. To clear this problem, create the holes no each leg separately. Get the Model file by visiting the following link:-http://bit.ly/2ogQDSk
Key of Iron Safe (Autodesk Inventor 2013)
Serial No. 212 Key of Iron Safe (Autodesk Inventor 2013) Click the following link to get the model file: –http://bit.ly/2nSa3N5
Create a Twist Drill as an ‘iPart’ through-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 211 Create a Twist Drill as an ‘iPart’ through-Autodesk Inventor 2013 (with caption and audio narration) iParts are different from standard parts they are table driven part factories with a group of parts. The parts have the different parameter and different features that are controlled by table. The table is controlled by iPart Author or Spread Sheet. Click the following link to get the model file: – http://bit.ly/2mXVsjd Transcription of Video Activate the ‘Create iPart’ command. iPart Author dialogue box is visible in the graphics window. Notice that columns for the named parameters were automatically displayed and iTwist Drill-01 has been added to the current file to define the first family member’s part number. Only 3 named parameters are required, so discard the other parameters by clicking Remove arrow button one by one each time. Right click the row of iTwist Drill-01, and click Insert Row in the context menu. In the second row change the value of diameter Major, Overall Length and Flute Length for the new member. Click OK to generate the iPart. Parameter Table has been added in the browser bar. Click the ‘+’ sign to expand the node. Right click the iTwist Drill-02 node and choose ‘Activate’ option to change the size of the member. Activate the first member once again. Right-click the table icon and select ‘Edit via Spreadsheet’. The iPart table is opened in Microsoft Excel. More parameters can be added with the excel file. Save the spreadsheet and close it. In the browser bar, expand the table node, the family members have been automatically added, it can also be seen from the Edit Table. Save the part file.
Modelling a Bolt and Nut in Creo Parametric
In this tutorial we will create Bolt and Nut by utilizing part modelling and assembly modelling capabilities of Creo Parametric 2.0. To animate this assembly read a related post. (Animation of ‘Bolt and Nut’ || Using Creo Mechanism) Viewers will be able to watch application of many part modelling tools like Extrude, Revolve, Helical Sweep, Chamfer, Mirror and Section Views along with 2D sketching techniques and utilization of assembly mates. Transcription of Video Create a new part file utilizing the default template and enter the name of the model ‘Bolt’. Start a new sketch over ‘Right Datum Plane’. Orient the sketching plane parallel to the screen by clicking Sketch View icon. Clear the screen by closing the visibility of Datum Planes, Axis, Points, Spin centre, etc. Activate the Circle tool and draw a circle along with dimension as displayed. Exit from the sketching mode and switch to Annotate Tab. Activate Show Annotation Tool and select the sketch. Applied dimension will be highlighted. Turn on its visibility by placing a checkmark in the show annotation dialogue box. Apply and save the changes. Select the dimension in Model Tree and open its property from the context menu. Change its display name to ‘D’ and apply changes. Switch back to Model Tab and activate Switch Symbol Command from the Model Intent Panel. This will display names of dimension in place of values. Re-edit the sketch. Convert this circle into construction geometry. This dimension sd0 or D will now onwards be used as a reference dimension and almost every new dimension would be relative to this dimension. Activate the Sketcher Palette and find the 6-Sided Hexagonal shape. Double click its icon to insert it in the active sketch. As soon as the 6-Sided Hexagonal shape is inserted in the active sketch the Rotate and Resize tool would be active. Move the sketch towards the intersection point of reference lines and rotate it 90 ° in an anticlockwise direction. Add a new dimension on this Hexagon by delegating the conflicting sd1 dimension. Fill the dimension values as displayed. The sketch is complete so exit from the sketching mode. Activate Extrude Tool and select the sketch. Change the extrude direction and fill the extrusion depth value. Execute the command. Save the model file. Change the colour of the model as per your choice. Create a new sketch over Left Face of the model. First specify new references, with which new sketch will be constrained to. Draw a circle tangent to these reference lines and finish the sketch. Create a new sketch over Front Datum Plane. Take the project of circle drawn on last sketch. Specify new references and draw the sketch as displayed. Delete the unnecessary lines and apply the dimensions as required. Finish the sketch and hide the visibility of sketch 2. Activate the Revolve tool and select the sketch. Now select the X axis of coordinate system to define the axis of rotation. Specify remove material option and execute the command. Start a new sketch on the Right face of the model and take the project of the circle drawn on sketch 2. Delete the projected sketch but you can see its reference is still present there that would be used to dimension new circle. Create a circle and add the dimension as displayed. Finish the sketch and activate the Extrude Tool. Select the sketch, then enter the depth value of extrude and execute the command. Start a new sketch on this face of the model and draw a circle with the dimensions as displayed. Extrude this sketch with a depth value of 2 inch. Activate Edge Chamfer Tool and set the dimension scheme to angle and distance. Fill the values in the input boxes, select the edge and execute the command. Switch to view tab and activate section along Z direction. Open the file named unf_external_thread_profile. Here you can see a sketch profile is drawn. The pitch of the profile is 1/20 inches which governs all the other dimensions by some relations. Copy the sketch present in the file and return to the previous file. Activate the Helical Sweep tool. Now define the Sweep profile for the Helical Sweep. Draw a sketch over Right Datum plane. Define the new references and draw a Center Line. Draw a line, the length of this line would be length of the thread. Exit the sketch. The tool has not selected the internal Center Line as axis of revolution so manually select X axis of coordinate system to define the axis of revolution. Activate internal sketcher to create the sweep section or profile. Place a Geometric point on the intersection of reference lines and lock it. Now paste the 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 and rotate the profile -90°. 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. Add more constraints and lock the dimensions. Apply some more dimensions to move the sketch at the required position and exit from the sketch. Specify the pitch value as displayed. Activate the remove material option and execute the command. Supress the section view. Save the file. If you change the dimension sd0 or D in the sketch1, the model will change accordingly. Create an axis parallel to the X axis of coordinate system. Save and close the file. Start a new part file and give it the name ‘Nut’. Start a new sketch over ‘Right Datum Plane’. Create a circle and apply the dimensions as displayed. Exit from the sketching mode and switch to Annotate Tab. Activate Show Annotation Tool and select the sketch. Applied dimension will be highlighted. Turn on its visibility. Open the property of the dimension and change its display name as ‘D’. Display the names of
iTwist Drill (Autodesk Inventor 2013)
Serial No. 210 iTwist Drill (Autodesk Inventor 2013) In this part modeling 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 mathematical relation between the dimensions applied in the due course of modeling the ‘Twist Drill’. Parameters used in iTwist Model with Autodesk Inventor 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 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 drill bit. The process will be the same as applied earlier. Later more coil feature will be applied to complete the model. Features applied in creation of iTwist with Autodesk Inventor 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 following video to understand all the process clearly Click the following link to get the model file: – http://bit.ly/2mVhfIk To properly understand the creation process of an iParts in Autodesk Inventor, read the related Blog Post mentioned below…. Create a Twist Drill as an ‘iPart’ (Autodesk Inventor 2013) And to more understand twist drill geometry watch the following image and visit the associated link.. TWIST DRILL GEOMETRY.
Handle of Tack Hammer-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 209 Handle of Tack Hammer-Autodesk Inventor 2013 (with caption and audio narration) Here we focused on the design of handle of Tack Hammer (also called Upholstery Hammer), since the design of hammer has already being discussed in our previous video named ‘Hammer’, so it is not described here. Click the following link to get the model file: – http://bit.ly/2nMONbS Transcription of Video Open the Assembly file of ‘Hammer’. A pre-constructed Part1 file is placed in this assembly. Create a new component with an English template by using Create Component tool. And change the name of file Part2. Select the back face of the model as a base plane for creating a new component. Create a new sketch on this face. Turn off the transparency, so we can see the Part1 more clearly. Use the Project Cut Edges command to get the model edges. Convert all the projected lines into the construction except to this rectangle. Create a base sketch of handle with the given dimensions by utilizing line, circle and arc tool. Now the sketch is complete, exit from the sketching environment. Activate the Extrude command. Select the each individual profiles. Set the value in the distance field. Click OK to execute the command. Close the visibility of Part1 and Work Plane1 to see the Part2 (handle) more clearly. Change the colour of model to ‘Birch – Solid Stained Light No Gloss’. Open visibility of Sketch1 in the Extrusion1 feature. Create a new sketch over the front face of Part2 to create a wedge on the handle. Take a project of the rectangle by using Project Geometry tool. Finish the 2D sketch. Close the visibility of Sketch1 in the browser bar. Activate the extrude command once again. Fill the value in the distance field and execute the command. Return back to the assembly environment. Open the visibility of Part1 to complete the assembly. Check the interface between Part1 and Part2. Save the Hammer assembly.
Door (Panel with Frame) modified design–Autodesk Inventor 2013 (with caption)
Serial No. 208 Door (Panel with Frame) modified design–Autodesk Inventor 2013 (with caption) This video tutorial features the designing process of a Door (Panel with Frame) with the aid of Autodesk Inventor’s part and assembly modelling functionality. Here we have added some more feature i.e., design of rounded beading, cutting of rectangular slots around the Frame of Panel in our previously created model. The highlight of the video is application of ‘Copy Components’ feature that is quite a time saving utility available in the Assembly modeling environment. Click the following link to get the model file: – http://bit.ly/2nHK1w6 Transcription of Video Create a new assembly file with an English template. Place the Part 1 and Part 2 in the assembly. Apply constraints between Part1 and Part2 to position properly according to the design of the frame. Two more instances of the Part1 and Part 2 are required, so use the Copy components command to duplicate these parts. Activate the Copy Components command. Select the Part1 file to create its copy. Take a look on this green status button which is active by default, it means a copy of the component would be created that would not be associative to the source file. Click Next button. Click OK to generate the new component. Unground the Part1_CPY to apply the constraints. Rotate the component to position properly for applying new mates. Apply Mate and Flush constraints between Part1_CPY and Part2, so that the parts may fit with each other without any obstacle. Check the interface between Part1 and Part2. Also create a copy of Part2. Apply the mates as shown earlier. Now the assembly is complete. Save the file with the name Subassembly-1 and close it. Open the Part3 file from the Subassembly-2 folder. Draw a new sketch on this face to create the beadings with the aid of Project Cut Edges command and Arc tool. Activate the Extrude command and select Cut option to remove the extra material. Activate the Mirror Tool and select the Extrusion43 feature from the browser bar. Define the XZ plane of the model as a mirroring plane and execute the command. Create a Work Plane at a defined angle with respect to this edge. Start a new sketch over this Plane. Use Project Cut Edges command to convert the intersecting edges of the model as sketches. Exit the sketch and activate the Extrude command with Cut option to remove the excess material from the model. Remove the material from this face as done earlier. Repeat the same type of operations which were done earlier. Mirror these three features by using the mid plane of the model. Create a new work plane on this point perpendicular to this edge. Create another work plane at an offset distance of 1/16 inch from this work plane and close its visibility. Create a new sketch on the Work Plane30. Use Project Cut Edges command to get the model edges. Draw a rectangle with the given dimensions. Exit from the 2D sketch. Activate the Extrude command with Cut option to create rectangular slots around the rounded beading. Mirror these extrude features to complete the file. Save the Part3 file and close it. Open the Part4 file. Draw a new sketch on this face to create the beadings with the aid of Project Cut Edges command and Arc tool. Activate the Extrude command and select Cut option to remove the extra material. Activate the Mirror Tool and select the Extrusion25 feature from the browser bar. Define the XZ plane of the model as a mirroring plane and execute the command. Create a new work Axis by using these two points. Create a Plane at a defined angle with respect to this axis. Start a new sketch over this Plane. Use Project Cut Edges command to convert the intersecting edges of the model as sketches. Exit from the sketch and activate the Extrude command with Cut option to remove the excess material from the model. Mirror the Extrusion26 feature by using XY plane of the model. Create a new sketch over the front face of the model. Use Project Cut Edges command to get the model edges. Draw a rectangle with the given dimensions. Exit from the 2D sketch. Activate the Extrude command with Cut option for making slot over the beading. Mirror the cut feature by using XZ Plane of the model. Save the Part4 file and close it. Open the Part5 file. Repeat the same process as done earlier in the Part4. Now the model is complete. Save the Part5 file and close it. Create a new assembly file with an English template. Place the Part3 and Part4 files respectively by using Place Component tool. Apply the Mate and Flush constraints between these two components to fix it according to the design of Door Panel. Check the interface between these components. Place the Part5 file. Fix it in the same way as the Part4 was fixed with Part 3. Place another instance of the Part4 in the assembly by using Copy Component tool. Fix the Part4_CPY into the groove of Part3 by using mates. In the same way, place second instances of Part5 and Part3 and fix them to complete the frame. Place the Part9 component in this assembly and fix it inside groove of the frame. Place one more instance of Part9 in the assembly and fix it tending towards its completion. Place Part10 component in the assembly and fix it by applying mates. Check the interface between Part10 and Part3. Save the assembly with the name Subassembly-2. Create a new assembly with an English template. Place the Subassembly-2 file. Copy this subassembly by using Copy Component tool. Change the name of the newly created subassembly as subassembly-3. Utilize the ‘User Path’ option to define a new save location for Subassembly-3 along with its related components. Fix these components by applying Mate and Flush constraints between them. Save the assembly with the name ‘Subassembly of
Photo Frame (Design-2)–Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 207 Photo Frame (Design-2)–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/2ouarlz Transcription of Video Create a new part file with an English template. Start a new sketch over XY plane. Draw a sketch with the help of Line tool and apply the dimensions as displayed. Use constraints to position properly and fully constrain the sketch. The sketch is complete, hence finish it. Activate the Extrude command and set the direction arrow to ‘Symmetric’ option. Enter the Extrude length and execute the command. Change the colour of model as your wish, so that it can be seen clearly in the design window. Save the file with the name Part1. Create a Plane at an angle with respect to this edge. Start a new sketch over this Plane. Use Project Cut Edges command to convert the edges of the model as sketches. Exit the sketch and activate the Extrude command to remove the excess material from the model. Create the same type of cut on the other side of the model, by utilizing the Mirror Tool. Activate the Mirror Tool and select the Extrusion2 feature from the browser bar. Define the XY plane of the model as mirroring plane and execute the command. Save the file and close it. Create a new assembly file with an English template. Place the Part 1 in the assembly. Save the file with the name Photo Frame (Design-2). Activate the Copy components command and select the Part 1. Take a look on this button which is active this time, it means a copy of the component will be created that will not be associative to the source file. Click Next button. In the Copy Components: File Names dialogue box, remove the check mark from the ‘Suffix’ option and give the name of the new copied component manually. Edit the Part2 to resize the model. Return back to the assembly environment. Unground the Part2 to apply the constraints. Apply Mate constrain between side faces of these two parts. Apply Flush Mate between top faces of these two parts. Apply another Mate constrain between vertical edges of each two parts. Check the interface between two parts. Activate the ‘Copy Components’ tool once 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 position it properly for applying new mates. Apply the same set of mates as shown earlier. Now create a copy of Part2 in the assembly and position it properly. Apply mates between the components to complete the model.
