I have tried to create attached drawing in solidworks using sketched bend option ,i could not match the given dimension in drawing.
can anyone help me to resolve this issue
Erik and Paul Cullen are correct in their calculations and that you must do more research into your bend allowance if you wish to do your calculations manually. However, letting SolidWorks to do it would be much easier. I have included a process below to create your sheet metal part if you know your starting sheet dimensions and wish to go from there (instead of creating the part and trying to get it to be the correct length).
As a note my dimensions in my process are set to inches by default but you should get the idea.
I start off by creating a sketch to make my flat sheet metal piece. In this case I assumed the piece was 150" x 150" but you can change the dimensions to whatever you need.
Next I used the Base Flange/Tab button to extrude the sketch. In this case I made the sheet metal piece 3/16" thick.
I then created a sketch on the top surface of the sheet metal piece and created two lines in the sketch. Each line will represent where I want to bend my base piece. As Paul Cullen and Erik pointed out, if you want to get the dimension correct the first time you must know your bend tollerance and thickness. However, what I usually do is set the dimension to the ideal amount and then fine tune it if need be after. Using the sketch I have create I can now use the sketched bend feature to bend the metal base.
I selected the center of the sheet metal as the part that I wish to remain fixed and made sure that the bend direction and angle was correct. The result is seen below.
As you can see, my inital guess with the 10" dimension was not 100% accurate to have an overal bend length of 10". Instead I forgot to take into account the material thickness and I have an overall bend length of 10 3/16". This is okay though cause now all I have to do is change both original 10" dimensions to be 3/16" less and it will be correct. SolidWorks will calculate this for you as well if you simply edit each dimension and type 10 - 3/16.
Hopefully this answers your question. As I stated earlier, the process I should went through I use when I already know the original sheet metal piece dimensions that I have to work with. However, if I am more concerned with the final product and do not care about the sheet metal length or dimensions, then my sketch for the base flange/tab feature would be as you did in your ppp zipped files.
When I do sheet metal project similar to this I start with a sketch on a plane and dimension the sketch using the dimensions you have in your jpg. So I would make the side line 130 long and the top and bottom lines 10 long. You can use relations to make the sketch simpler to alter in the future.
From there, I then use the sheet metal option and tell it a thickness of 1.6. The important part in this step is to look at which side the sheet metal is being extruded on. Since your sketch was done using the desired outer dimensions you must make sure that your sheet metal feature is extruding the part thickness wise inside.
thank for your info,in this case i want to use sketched bend option can you guide me how to do this..
Here's a pretty good video using sketched bends: https://www.youtube.com/watch?v=2NzfmGxsiM0
there is no information about sketched bend option in that video..
I want to know how to calculate the full length of sheet if i go for sketched bend option..
I have taken 150 mm full length sheet then i have drawn 10mm line in both side and using sketched bend option bend it but i could not match the 130mm and 10mm given dimension in that model.
can anyone guide me to calculate the length
I can walk you through how to do what you need but to best help you I would like to get some screenshots to put in the post. I can do this come Monday when I get in to work to help you through it. If you need to know sooner I can try to walk you through it without screenshots. Let me know.
I want to know how to calculate the full length for getting the given dimension
For your reference i have tried trial and error method .please go through the attachment.
The reason the sketched bend does not calculate correctly is because you have not allowed for the material thickness or for any bend allowance. A quick calculation would be 10+130+10= 150 less (4 x 1.6 (material thickness)) 6.4 = 143.6 you would then want to draw your sketch lines at (10-1.6) 8.4 mm instead of 10 mm. You would then need to measure the part you have created and adjust your sketches as required to get the correct size of part. See attached part "Sketched Bend"
It is easier and quicker to create a 3 line sketch as Paul had said and then extrude the base flange, see attached part "Base Flange" as SolidWorks automatically allows for the material thickness and calculates the bend allowance / bend deduction / k factor for each fold.
Thanks for your answer,is there any standard formula for calcuating the full length for sketched bend or else we have to follow trial and error method.I have tried your method its coming correctly but small deviation is there . one more clarification in that equation you have used 4 how you get that
There are standard formula. I have a spreadsheet somewhere that I used to use, but letting SolidWorks do the math (I.E. model your part in the formed shape and let SW generate the flat) is really much more straightforward and I haven't manually calculated a flat-pattern and/or bend locations in long while.
If you Google "sheet metal bend allowance" you will find many good explanations of bend allowance and flat-pattern calculation. Much faster than I could find my spreadsheet.
Help in SW also has as pretty good explanation K-factor and bend calculation, look in Sheet Metal, Using Sheet Metal Bend Parameters.
Thank for your help to solve the issue.
I got the exact answer, with help of your suggestion. Thank u all
For your reference I've attached an image.
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