SheetMetal not able to make a box correctly - please help

[Anonymous]

Hi, the long awaited Sheet metal functionality looks very cool Thank you sooo much for getting it published and released to the public

I do have an issue and not sure how to get it to work correctly Please see attached photo and .f3d file. the problem is that when making a simple box the corners are not generating correctly as i would expect for a sheet metal box to look like. in the corners it is cutting out a 0.60 size area at the root of the bend and i don't understand why. i have tried changing all the settings when making the flange but no use. tried the bend overrides but no help, if i put a value less than the radius (0.06) it just gets ignored, if i put 0 it gets an error i just cant get the two sides to come together as you would hope it would. Material is 0.060, 16gauge CRS

Thank you for any help in advance

Regards

Mitch 

[Anonymous]

I tried to upload the .f3d file and the website tells me it is not a valid .f3d file so i uploaded the .step file

[TrippyLighting]

Try again please. I've uploaded tons of .f3d files.

[Anonymous]

testbox file upload retry

[Anonymous]

upload is working now
Thank you

[Anonymous]

just uploaded another pic of the issue. need to get the sides to close the gap.. Please see pic

Regards

[Anonymous]

More info i have found on this issue,

One thing i found is that if i use the flange command and select all 4 sides at once then i do not get the large gap but if i select one edge with the flange command and complete it with the ok button then do another flange command and select another one of the edges then i get the gap. the problem if i select all 4 at the same time then all 4 sides will have to be the same length so if i select one side and do flange and make it 1" then select the next edge i get the large gap. i was watching the video "Sheet Metal Progess" from Jul 1, 2016 link is -> www.youtube.com/watch?v=BEDtSreoXe4

It has a lot of good info on making a part from sheet metal and did not seam to get the gap issue but is also doing all 4 sides at once.

Regards

Mitch

[HughesTooling]

I suppose a workaround would be create all the sides at once to the same height then use press\pull or move face to change the height of the individual walls.

[Mike.Grau]

Hi @Anonymous, @HughesTooling, @TrippyLighting,

Thanks for your Post in the Forum.

I guess you might look for a design like this.

Please, feel free to use the design here

I hope this helps.

Thanks,

[Anonymous]

Hi Mark, Thanks it is a good workaround, but i think Autodesk should fix the issue, I did notice that the miter check box has direct impact on the corner but it is not available if you are just working on one side, also even if i do all the sides at once and adjust with press pull the flat pattern is not really correct.

 

Thank you for the input

Regards

Mitch 

[Anonymous]

Hi Mike, thanks for your input, I was able to get that far the issue is the flat pattern and the gap at the bottom of the model. I guess if you are just going to make a drawing and never make the box for real it is ok but to have a plasma/ Laser cut it out then it will be a big issue. I can lay it out by hand and ignore all the errors but it would be nice if it worked correctly as it should and make it as if someone was actually going to produce a part from it.  there is a big difference between concept and reality.

Regards

Mitch 

[HughesTooling]

Hi Mitch

Can you point out what's wrong with the flat pattern please, I don't know that much about sheet metal and not sure where the problem is.

I've also made a post here with some observations on the problem caused when you can't create all the flanges in one go.

Mark

[Anonymous]

Hi Mark, so i have added two pics to show what i am talking about. the first is what i would think it would create and the second is what it is creating. also if i could take the miter option and use it like a tool from the tool pallet to join individually  created flanges that would also help to some degree. 

[Anonymous]

Hi Mark, Great post!!  i also wanted to add to the pile - how would you create bend tabs if needed and i haven't even mentioned adding hems - used a lot in sheet metal bending. as a note also looking at the way it is making some of the corners, it can make sense in certain situations where that corner type could be used but i think it would be using very thick martial and stamped brackets...

     

[innovatenate]

It seems like you may be after creating a box with a 0" bend radius. The does not appear to be supported at the moment, but I am able to override the bend to .001 inch, which is pretty small and make for almost a sharp corner.

The rule of thumb I understand is that the minimum bend radius should be equivalent to the material thickness. Otherwise, the material will be compromised when formed, you'll get cracks in the material on the outside radius along the bend.

I sketched out an illustration that highlight where the start of the bend line, and the bend center are the bend would start occurring in multiple directions. With the flat pattern solver, it tends to only like bend in one direction. So this overlap area is a problem. In the case of a 0 radius, then what you're proposing would be doable.

 

However, with bend radius, some compensation has to be made for the length of the flattened material required for the bend. A corner like this can be made with the trim to bend option in the 2 bend corner override.

This will yield a flat pattern like you've drawn:

With that said, you can get pretty close if you override the bend radius to a really small value like .001. Then you'll see a corner like this:

And a flat pattern like this where the relief geometry is so small that it isn't detectable unless you zoom way in.

I've attached a sample file for your reference.  Does this help or am I overlooking something?

Thanks!

[Anonymous]

Hi Nathan, Thanks for the response, I had not changed the bend radius to less than the thickness of the metal. To do so i would end up with errors in the total calculation. For me the whole purpose of using fusion 360 to do sheet metal is overall flat development.  for instance in a simple box that is 2" square with 1" sides. to check if fusion is able to calculate the correct bend allowance and line placement and overall size of the metal to cut. So with a 2" box like i described the 2" X 1" will be considered the mold line size. to make a 2 X 1 box from metal will require that i cut a piece of metal that is a total of  3.791 X 3.791 - using 16gauge CRS (Cold Rolled Steel) sheet. that is 0.060 thick , then the first bend will be placed at 0.948 from the end on all 4 sides and the center area should measure 1.896. If bent correctly that will give us a 2" square box with 1" sides measured from the outside surfaces. So to change the bend radius to .001 will give the wrong calculation and the box will not be the correct size after bending. Currently i have been using fusion to draw out the flat development but doing the calculations out side of fusion and that works ok but is very slow. Also the bend table is kind of lacking. here is an example of what i think would be more useful

       

Thank you for the input but realize  that is not a visual issue it is a functional problem - Please let me know if any ideas to get this right.

Regards

Mitch

[Anonymous]

I just wanted to add if you look at the calculations from the last post there are very close to what fusion is calculating but the cut lines for the sheet are off due to the way it is making the corners.. to get this drawing i created the Flat pattern from the model and then used it to make the drawing.

[innovatenate]

We know bend tables are light at the moment. There are further enhancements in the making, the Fusion 360 Ideastation is the best place to request feature enhancements. There is one feature I really like, though. If you drag an bend ID annotation, a leader line is added for you automatically. 

When you say that "the cut lines for the sheet are off due to the way it is making the corners," I'm not sure I follow what is expected versus what is happening. From what I gather, you're expecting relief cuts to be different then what is currently available. Looking through our help, I think we could do a better job explaining what the various relief options do and what to expect. However, if you take a look at the Inventor help, there are some good parallels between Inventor and Fusion. 

Inventor help:

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2016...

I've consolidated it down in the below image for reference.

To my best understanding, using the Tear option with the miter selected is the closest option available.

The bend radius and the K-factor will make a big difference in the overall dimensions of the flat pattern. Adjusting these two parameters in the sheet metal rules will alter the outcome bend allowance generated in the flat pattern.

As far as I can tell, everything is working how it is designed to work. Hopefully this helps some. Thanks in advance for any clarification you can offer.

[HughesTooling]

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@innovatenate I thought I'd have a go at the box with the tabs in @Anonymous post above and found a problem. If you make the flanges touching the other sides of the box they combine!

You can workaround the problem by setting the angle to 90.01° but I think there should be some way of doing this without cheating. Have I missed something and should I make another post to report the problem?

I've attached a file with the best I can come up with for the box above.

Mark