Can anyone help me to flatten this Surface

[ptc-6654839]

Hi everyone can anyone tell me how to flatten this surface?

I tried but it is failing....can anyone tell me the reason?Thank you.

I am new to this community.

[TomD.inPDX]

Welcome to the forum, Jimit.

This is a coined plate and in Creo, this is a form feature. Creo doesn't account for thinning in forms.

Sheetmetal parts (not the application) depend on a formulation to calculate how much material stretches and crushes in the form operations. This is known as K-factor or Y-factor. There are some specific dependencies on these values depending on how critical the task is. Creo does its best to approximate this in one of several methods. if you use the sheetmetal application, it needs ot know the thickness and the y-factor or k-factor. Your part does not yet have a defined thickness, which is required for a sheetmetal unbend/flat pattern feature.

Due to the odd angle of the radius, this part is a bit fussy in the sheetmetal module. I am going to assume the outside of the metal is clamped when stamped and coined. That means that all the material is stretched to make the "dished" segment. I also have to assume a material side and thickness. I will create a video of how this is done in Creo 2.0. This will give you the basic concept, but you will need to adjust the bend factor.

The form is done separately. But for now, I can get you to a flat pattern... Let me make the video.

[TomD.inPDX]

I am surprised i got this to work with a quilt form. It was backwards from what I was thinking but it works if your material thickness is reasonable considering the radii provided in the original IGES. I reduces the thickness to .001 from what the video used (meters is the IGES default).

The original IGES doesn't work for the quilt so I did a zero offset quilt from this. For some reason, this worked. What was more surprising is that the unbend feature worked while preserving the form. Good news because this is useful for making the coining die. I knew it should be able to do this, but would have liked to make the form in the flat and use the bend back feature. That didn't work through a bend.

Full version Creo 2.0 attached.

[TomD.inPDX]

Just for completeness...

[ptc-6654839]

wowww thanks a lot sir...today i have learnt so much from you ...i was struggling with sketched form...i wasn't able to give proper radius at the intersection of side and bottom face.

[ptc-6654839]

and i think the second video is much more accurate than first one ....

[TomD.inPDX]

The second video is a continuation of the 1st but I did change the thickness. If the material was too thick, it would not form because the radii went to zero. Each time I try these challenges, I learn something new. I am happy that the model with the Form Feature still flattened without any special consideration.

There are several methods by which this can be created. I used a large punch die to make the blank but the form die becomes special to account for the formed region. The second method would use the depressed area as the master where the which is 1st formed into the "U" shape and then a hem tool to create the offset. One hint that this was not the case is that the radii of the form are not concentric with the radii of the edge. Both methods are equally valid in the shop but one has much more tooling expense.

In practice, yes, metal will deform and accommodations have to be made for "bunching" when you use a form tool in both cases. Creo does not account for material thinning due to stretching or wrinkles due to bunching. Other than extreme precision designs, the variation is easily tolerated. The tool and die makers are magicians in their own right.

The point is, you can reverse the process by working from the inside and the overall size will be slightly different. This would be the case if you use a hem tool to create the "S" shaped lip.

In practice, as a designer I do not provide flat pattern data to the fabrication shop. I may reference it to make smart decisions, but the final bend factor details I leave to the shop so that they meet my final part requirements. The manufacturing process is a level of documentation outside my control. There the smallest of details will be determined.

[ptc-6654839]

yeah but in second video length varied than in 1st video.Ohhhh i try ur suggestion for modeling method. Yeah i read creo doesn't account for flattening form tool. So what you do is give your model to sheet metal guy and they carry out their own calculations?:O .. This is my very first project in sheet metal and some terms i am hearing for the very first time!!!..

[TomD.inPDX]

True about the 1st length vs the second. This is what the bend allowance does. Google that and it will make sense.

Manufacturer's calculation can also be doing a sample and analysing the results. They make adjustments according to the first article results. They are pretty good at it

[ptc-6654839]

hahaha ok ...but that would be interesting to know right? whether our calculation and practical lenght matched or not ?...do you have some complex examples where you calculated and got almost same answer ?

[ptc-6654839]

and can u please send that part file ?

[TomD.inPDX]

Creo 2.0 full version attached

[TomD.inPDX]

I never need to know. I have had shops tell me to simply use a k-factor of 0.4 and all is good if I -really- wanted to know. The actual form die used and true bend radius all affect the overall length. General shop practices for sheetmetal is +/-.015" across a bend; edge to edge, +/-.010"; and location on a face +/-.005. As long as my design can accommodate this level of accuracy, it is no issue. this is for typical sheetmetal boxed using .03"-.093" material thickness in the size of rack equipment (20"x20"xn). Looser radii have less crush... coining dies have more stretch. I don't really care what dies a shop uses but they know how to account for them.

The times I use the sheetmetal module is to unfold a part to see the flat pattern of odd shapes. This lets me make good decisions on cuts or tool angles for efficiency in setup. When I do cylindrical work, I use angle references on the drawing rather than linear dimensions on flat pattern views. So whatever the true length is, the angle determines the feature position. The rules I live by is to make the design flexible to accommodate the shop standards. I know when I ask for something special that I will pay for that.

Remember that they also need to overbend to achieve the final angle. All this has to be accounted for in tooling. To get a true 90 degree bend, you might be creating an additional expense in your tooling or process. They will need to overbend this by about 2-3 degrees to get a perpendicular.

[ptc-6654839]

but i have seen in many case ..or say take this case...if you are referencing with angles...then i have very odd angle of 3.15 degree...i mean that is not measurable apparently...instead i contrainted it with radius and length...Ohh is it so? i mean in every case the do overbend?and thanks a lot for part file

[TomD.inPDX]

Yes, all metals spring back on a conventional break die but can be minimized with coining dies.

Again, I am not aware of your use case or the overall design. Making this cost effective would have me conversing with the manufacturer(s) for the best solution. A lot of factors to consider.

Cylindrical designs is the only place I typically use a flat pattern on a drawing and the position of features are almost always required at a specific angle in the formed state. As a designer, I detail design intent. The fabricator is responsible to deliver to that requirement. My responsibility is to make sure the fabricator can meet my requirements within reason (allowable tolerances and minimized secondary machining).

[ptc-498403]

Excellent coverage Antonius! Especially the fabricator involvement. Done hundreds of press brake ops using .4 and the shop was always able to compensate for material diffs. No wonder your are platinum and thanks for helping many folks!

[ptc-6654839]

okkk thanks a lot sir for helping out

[bduncan]

See the gif.

[ptc-6654839]

i don't what i did wrong when i was flattening with flatten quilt...this option is not working out for me.

[ptc-6654839]

is there any rule for selecting the origin for flattening?

[TomD.inPDX]

Flatten Quilt is a touchy feature that does do some wierd things. If you are an expert with it, you might fine tune it to control the deformations.

If you want to try what Blue Duncan did, 1st change the units to inch, lbs... etc.

Open the options dialog and use the ADD button and enter Option Name "new_flatten_quilt" and enter the Option Value as "yes".

Now the dialog for flatten quilt will be different. Select the quilt (right click until it all highlights and select) and select a vertex.

A preview should pop up after a few moments of thinking. If not, pick a different vertex.

[TomD.inPDX]

Nice Blue. I couldn't get this to work. Did not try selecting all the surfaces, though.

[TomD.inPDX]

That is the new flatten quilt dialog (new_flatten_quilt yes; hidden Creo 2 option).

This allows selection of surfaces rather than just quilts.

In Creo 2.0... at least mine, it fails even if I do it exactly the same.

Edit: never mind, it worked when I changed the units to inches and let the part convert

[ptc-6654839]

haha yes changing the vertex even helped .... i am loving this software ^_^ thanks again

[bduncan]

Using search tool can get more results that you want,I love this tool! I will do some videos for using search tool