if you draw a curve in a sketch then boss extrude it to the width you want, how do you get the degrees and bend lines for using a break press to make it?
Do I convert it to sheet metal?
This is a thin feature?
You can do the exact same thing with the base flange tool. Create your curved profile and then pick it for the base flange, that is the easiest way.
You can convert your existing part to a sheet metal part by clicking on the convert to sheet metal. Then you have some options you have to select. Pick a base face and pick the bend and you're all set.
Thanks, I will try it
where do you get the info on bending?
Typically you would get it from the flat pattern when you make your drawing however you can get some of the parameters from the model under the Cut list parameters.
Bounding Box Length is the Flat Length of the part.
Bounding Box Width is the Flat Width of the part.
Here's a quick (obviously it's bad) drawing:
I would need more bends the curve is 36". What I want is the number of bends and each degree of bend to make the curve. Usually I just cut the side plates and bend it to the shape.
It's 36" huh? At this point I think you're going to have to describe in detail what the part is. Since you didn't give any dimensions I just made my own part to try and mimic the screen shot you posted. It's pretty obvious that my part is thicker than your part, relative to over all size, and I did that on purpose so you could see what was going on. Your screenshot almost looks like a surface and I didn't want to post anything like that because then it's hard to see what faces I'm selecting, etc.
What's your process because that's going to make a difference. Are you step bending? Do you have a slip roller? Are you using some special tooling or in-house tooling? What are the dimensions of the tooling to be used?
The model that I have made and the model that you took a screenshot of show an arc for a single bend. If you, in fact, are hitting this part multiple times then obviously these models are incorrect, but if the part comes out so smooth that you could approximate a constant radius then these models are a good representation and you need to start giving SolidWorks some of your in-house bend information, whether it's a bend table or some k-factor.
I mean this as politely and respectfully as text can convey... Until you supply that information, it appears to be a futile effort to try and help you in regards to this situation. Regardless, I think it would be best if you take the time to learn more about this software, it's capabilities, and it's limitations.
As I stated in the previous post, obviously these dimensions are not correct as you have not supplied any of the information. I have also used exagerated dimensions to make the screenshot easier to view.
Is this closer to what you're looking for?
yes that is what I would like to do
Cool... now you just need to find someone fluent in telepathy/thought-transference.
I thought that was how you were able to figure out what I wanted. the shell is .25" thick x 48" wide and the other measurements are on the picture I changed it to 30" circle. The measurements dont have to be exact just the steps to do it would be fine. All I had was my blackberry earlier so I couldnt reply with much detail.
You have missed the most critical bits of information;
The included angle?
How many steps are acceptable?
If you want a smooth circle, a rolling machine would be better.
If you are are wanting a flatted circle created by bumping on a press brake, why not draw those flats to start with? (per Denny's last image)
Joseph Fluney wrote: I thought that was how you were able to figure out what I wanted.
Joseph Fluney wrote:
I thought that was how you were able to figure out what I wanted.
Nope, and even if it would be convenient to be able to read other people's minds, the consequences far outweigh the benefits in my opinion. There are just so many things in life that need not be said.
I just tried to envision all the different scenarios based on what you had described and guessed that this was most probable.
Kelvin Lamport wrote: If you want a smooth circle, a rolling machine would be better.If you are are wanting a flatted circle created by bumping on a press brake, why not draw those flats to start with? (per Denny's last image)
Kelvin Lamport wrote:
Hey Kelvin, always good to see your input here.
I'm guessing that the OP may not have access to a large slip roller and/or a "smooth circle" is not required for this part. I'm also guessing that the OP was under the impression that SolidWorks would do this automatically.
From my experiances, there are a lot of VARs that purposely mislead utilize marketing in an effort to portray their product as something that can save the world, stop world hunger, cure cancer, rescue ducklings attempting to cross the highway do everything a customer needs.
Here's the sketch I used for making the base flange. This is but one way to do it, and the most straight forward I think for explaining:
D1 is the intended radius that the combination of bends should come out to.
D2 and D3 are leg lengths.
D4 is the opening angle.
Here's a zoomed in screenshot of the interesting part:
D4 is the angle of an arc representing the bend radius of your die. This arc is tangent to both the leg and the flat space between your bends.
D5 is the angle of the line representing the space between your bends. This line is tangent to the arc mentioned for D4.
Take those two highlighted segments and perform a Circular Sketch Pattern:
So here's the kicker...
You have to supply the critical information for the part and how you intend on forming it, SolidWorks isn't going to do this for you and even if it did, you still need to provide information to SolidWorks in regards to how your material will react to your processes.
Once you have set up the sketch you can create your "thin" Base Flange just like in previous posts and you're all set.
Typically you don't want to have sketches with excessive detail like this, but this is a pretty straight forward way to do this. There are other ways, which include but are not limited to using feature patterns as well as forming from a flat and adding bends,
Thanks, I have did it other ways by adding sketch bends, usually I just go bend it to fit the profile shape I cut out and mark down my bends for future reference.
I think I understand your predicament...
Basically, you and your team know fully well how to produce this part. You guys have done it many times in the past and have your manufacturing process down. You have side panels that are cutout (laser/waterjet/plasma) and fixed (welded) in place and this part that I have mistakenly called a strap (because I didn't know the scale) is a liner of some sort. To make this part, you step bend based on your side panels.
The challenge here is that you want to try and document and/or modernize your process by modeling this assembly in SolidWorks. You know how to make the part, but you want to be able to have a model of it for drawings, etc. and if at all possible, come up with a more "scientific" approach.
Correct me if I'm wrong with any of this, please, because I am just guessing...
If what I say is correct then unfortunately the answer, to the best of my knowledge, is that SolidWorks may not be appropriate for this specific situation. It is a great program but it cannot read your mind without the necessary critical information. What it can do for you is give you a good model once you have provided it guidelines, and from this, help you to produce other similar parts. For instance, if you tell it that all bends need to be spaced by 3 inches, and your tooling radius is 1 inch, then no matter what angle you enter, SolidWorks will update your model and do the "work for you." The trick here is that you need to set up a good foundation within the software to get to the point that I think you are trying to achieve.
Retrieving data ...