Mounting Bracket || Creo Parametric Sheet Metal Tutorial
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- Опубликовано: 23 авг 2024
- 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.
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Transcription of Video
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1. Start a new Sheet Metal Part file from scratch with the default template and give it a name 'Mounting Bracket'.
2. Select the Top Datum plane and create a new sketch on this plane.
3. Click the Sketch View icon to orient the sketching plane parallel to the screen.
4. Activate the Circle Tool and draw the sketch with the dimensions as displayed.
5. Convert this circle into construction geometry.
6. Create a line in the sketch and duplicate it to the other side, using a centerline with the aid of Mirror Tool.
7. Draw a new line and repeat the previous process for this line also.
8. Create arcs between these lines by picking its centre and ends.
9. Duplicate these arcs to other side using the Mirror Tool.
10. Exit the sketch and activate Planar Tool.
11. Fill the thickness of the sheet and execute the command after selecting the sketch.
12. Change the colour of the model as per your wish.
13. Create a sketch over Front Datum Plane.
14. First specify new references, with which new sketch will be constrained and dimensioned.
15. Draw the sketch using the Line Tool as displayed.
16. Exit the sketch and activate the Extrude Tool.
17. Select the sketch and activate Extrude both side of sketch plane equally option.
18. Fill the extrusion depth.
19. From the option tab activate add bends on sharp edges command, which would be equal to thickness of the sheet.
20. Execute the command.
21. Activate Flange Tool.
22. Select an edge to attach the wall and then fill the length and angle of the wall.
23. In the similar way add two more flanges.
24. Activate the Flat Tool and first specify placement edge.
25. Execute the command after defining the angle and length of the flat.
26. Start a new sketch over top face of the model and draw a sketch similar to this one.
27. First specify new references and use Line to draw the sketch at the defined position.
28. Activate Bend Tool.
29. First define the bend line and then fill the bend angle.
30. Execute the command.
31. Again repeat the same process to perform another bend operation.
32. Hide the visibility of sketch3.
33. Select the leg created with the extrude tool in the model tree and activate Pattern tool.
34. Open the visibility of Coordinate System.
35. Set Axis as the type of pattern.
36. Select Y axis of Coordinate System as axis of rotation.
37. Enter the number of members to be patterned.
38. Leave the default 90° Angle between the pattern members unchanged and execute the command.
39. Save the file.
40. Apply a Chamfer of 0.125 inch on the each of the legs.
41. Activate the round tool and apply fillet of .06 inch on these edges of the model.
42. Create a sketch on the top face of the model and draw a circle on this leg with the defined dimensions.
43. Create a hole on the leg using this sketch and extrude tool.
44. Open the visibility of Coordinate System and using its Y axis pattern the hole 4 times at an angle of 90°.
45. Create a sketch on the top face of the model and create a point to define the position for the new hole.
46. Activate the Hole Tool and select the point.
47. Define the diameter of the hole and execute the command.
48. Pattern this hole 6 times at an angle of 60°using Y axis of Coordinate System.
49. The model is complete you can generate the Flat Pattern of the model.
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dear sir please tell me in which condition we have to make the tool in design the sheet metal. or not
It depends on the fabrication method. Suppose you are going to design a water container of a cooler which you have seen in common homes. Observe it you will find it is created with single sheet of tin. It is the example of sheet metal design. The flat pattern of designed part can be generated after modeling it.
On the other hand observe the LPG cylinder. It can not be created with sheet. It is a molded part so it can not be created with sheet metal.
RUclips Video Modeling Tutorials just give you an idea about designing products. You can learn application of software tools. Actual designing is done on the basis of CAM means manufacturing of models.
Yes sheet metal designing depend upon the manufacturing .
I am cunfuse bcs we can make the drawing by using the command,like extrude cut ,revolve etc.But we would make the tool instead of direct command.So please tell me how far we can directly use the command.in designing the sheet metal products
Your ultimate goal is that at the end you are able to generate the Flat pattern of the model. Any method you can use which is convenient to you. The Drawing sheet of flat Pattern will go to manufacturing unit not your designing history.
Sir actually we have given two interview when i design the product in front of him he say that you will be design in such a way that it will manufactur easily
Ya it is said that designing should be similar to manufacturing, That way is quite robust and re-edits can be done easily. Some times people say it Micky Mouse method but it is quite robust way. I am quoting the lines of the author of Mastering Autodesk Inventor Book. You should discuss this topic over official Creo Forum to get more suggestion from experienced. users. Check my channel's about page to get link of the forum.
This is so helpfull, seeing the coments i notice they dont understand you do it in many ways just to show us more skills, i appreciate that, thank you!
Thank you for the tutorial in bending in Creo Parametric, the use of different tools to get to the same conclusion is amazing, once again, Thank you.
It would be more useful if it was highlighted how using the different methods produced different results (notice the hole pattern's relation to the bends and the tab size in the top view at the end). It's possible to get the same result, but it takes more calculation than illustrated. BE AWARE OF HOW EACH METHOD CHANGES THE RESULTS!
Thank u sir.....this video very usefull to learn my knowledge......
just amazing..thank you so much
it is really good thanks
Thanks you so much sir
Nice video
Thanks so much for this tutorial great help !
***** can you do a video on how to to make airfoil for airplane wing please
When I attempt to make the second bend on the third leg, the base moves instead of the end of the leg. Anyway to prevent this/
Very good, one I observed, is not more simple to make array or mirror to "make" the others 3 legs ?
***** I did recently download of Creo and I'm beginning to study, study also Solid Works, SpaceClaim, but which I am most qualified is in Autocad and Inventor. Very good your publications, congratulations.
hi can you please teach me hw to use sweep and helical sweep command?waiting for your reply
very good
1:44 how does this menu appear ? also, at about 1:50 how do you make it so the dimension just appears like that ? thanks
At 1:44 you can activate by right click menu and at 1:50 there is nothing special.
@@3DSolidModellingVideosCreo right click does not seem to work. i will probably discover eventually, not a major concern. i figured out dimension move, thanks.
1:24 why is you default orientation different than mine? (i am using creo 2.0)
I have configured Default model orientation as Isometric from the Option menu of the software.
You can change it by going to Option menu---Model Display---Model orientation.
@@3DSolidModellingVideosCreo thank you sir
hi where i can find planer too?i am stuck after finishing sketch:(
after4:22 i am not finding planer tool i am using creo2.0 parametric.
Thank you sooo much sir:)i was doing mistake at 00:45 second :)thank you once again GOD bless you and i will ask you more question hope you dont mind:)
Incredibly complicated, so much work to create simple part. Creo is so far behind competition.
Why do you need a sheet metal for this
The motive to create this tutorial is to show application of various tools 💥 related to Sheet Metal not to show only a modeling process of a specific model.
Hello!
please reply anyone
no voice!!!