i am trying make this helical profile in sheetmetal and flatten it..How can i do this?
I'm at a loss for words Lingesh. I have studied your part and have no idea what your intent is.
here is the full model which is used as guide for flow of water.This will be placed in the annular space between two cylinders.And since it cant be made in full in one piece,we are planning to make pieces of 90 deg (1/4th of a revolution) and then join by welding.Here is the snapshot of the full model..
Hi. The flattening command doesn't apply for every geometry, like the one in your case. If you are planning to build that element you have to make it like an assembly, you should split the entire element in parts. My advice is to split it in pieces so when you put them together and look from above, the same part shouldn't cover itself. In my opinion, the easiest and cheapest way to make flatten is using sheet metal and then laser cut it.
I guess u didn't see my first question and the attached part.. Yes am doing exactly what you are saying, like split it into quarter of a revolution and then assembly by welding.. But that part "split in parts so when put together and look from above" didn't understand.. Also I request you to see the part attached with main Q..
hei'ya Lingesh Sangur,
not sure myself what your design intent is-
but I'm guessing the quarter sheetmetal flat pattern is the bug-
so here's my take on it-
and a sample assy
hope this helps- have a good'n kelef
Hi Kelef Man,
can you share that part?is it helical profile plate or simple flat round plate you used in the assembly?
the parts are helical, sheet metal
the att.zip file in my previous post has the full assy.
just click on the link to download-
unzip and open with SW15-
also attached here is the "Q1-BAFFLE.SLDPRT"
single quarter part- you can edit/rebuild
as your joints and end design requirements
ur assembly is exactly what i am looking for..but
actually my question is is it possible to flatten that helical baffle-Q1?I dont know how they fabricate these kind of helix profiles.is it possible to make it by any of sheetmetal proces like roling etc?
this is a sheet metal part file-
and it is a helical part-
you can inspect the individual elements
in the feature tree to see how this is accomplished
there may be better ways- maybe someone will chip in
you can flatten in the part file as indicated-
or in a drawing you can insert a flat pattern view
this part would be produced by profile cutting of the flat pattern-
and then rolled for the helix
This is an interesting issue for sure. I had originally came up with something that matched (fairly close) to what I was able to garner from your (Lingesh's) file. This has a helical sweep with bends on the ends (one up and one down). You are going to get a kick out of it when you see what I had to due to get it to unfold. Then I saw Kelef's concept of this and realized that you probably wanted the legs going the same direction so you could put one end to end and end up with any total helical shape length you wanted. I gave up at this point (got lazy).
I have seen on "How it's Made" a slinky style spring from a single straight strip of sheet metal and winding it. Very impressive.
I decided to attach a file of what I had come up with which closely resembles Your quarter turn sample (with legs) and flattens. It is helical but not quite the same twist but darn close. This is an assembly file with your original and my part laid on top of each other so you can check out the difference. You will have to go from formed to flatten using the configurations in my part.
I saw the concept "leg up and leg down" in the original post-
not too sure of the welding on 90 degrees directly above each other
I would have probadly looked at maybe staggering/offsetting-
the kicker really is to turn it into lego type fully interlocking-
with as few unique components as possible- just a thought
have a good'n kelef
You have impressive conceptual abilities.
failed designer- over design everything
went on a couple of visits to Ikea- to learn to think
simpley and compact
Hi Dennis BaconKelef Man
I saw your discussion. As i said its used as a guide for the flow of water between two cylinders annual space.and if we use those legs up and down,it will obstruct the flow of water.Also kelef, the part you shared is helical,thats correct.but flatten part is not perfectly flat.its still some curved(formed) kind of profile.My intention is to give blank arrangement in a flat sheet. please the image of flatten and unflatten views,and also my intention of blank arrangement.Please correct me if my understanding is wrong..
I appreciate you guys and this forum as a whole..
I disagree Lingesh. The flat pattern is flat just not normal to your XZPlane. The reason for this is the profile was begun normal to the Helix which tapers upwards. I had no trouble adding a new plane on this and if it was not a flat surface I would be unable to do this.
Hi Dennsi Bacon,
Yes, now i realize my mistake on this..I didnt think it that way..Yes,on non flat surface plane creation is not possible..Thanks..
What I don't get, is why it seems so important to flatten it. In a sense, it almost already is flat. Unless you plan to stretch it out a lot, which I don't see in your assembly picture, the difference in Ø would be negligible, no?
I'm building something similar, then again, not. I plan to stretch out a lot more than you.
This is what I need; OD = 23"
I am ordering 5 parts like this;
Well, actually, more like this;
See, not even sheet metal. I just use top view, for drawing view, cheat the system with a configuration for side view, send top view to dxf for laser cutting... I cut in a 1/16" slice where the bend starts.
The real question is not how to get the right drawing and the real flat-pattern, I think that for real life, nobody will see the difference. The real question is how to go about stretching it out in real life evenly.
Our idea is to first weld all five parts together, end to end, while still flat, then use hydraulics to stretch it out slowly while welding in plates to keep it going even. Whole process should take about a half a day.
The real problem is not that I might lose a few thousands of an inch on the OD by stretching out, (if it really bothers you just test one part in real life then adjust the drawing,) the real difficulty is going to be welding the parts in perfect concentric.
As for the double folds, why fold it at all? In real life, you plan on giving it the part the helical form before or after the folds? I'd just weld the legs on after and actually use the legs to help to give all your parts the same helix.
Hi David Dessaints,
can you share the file here for better understanding?
my problem is i dont have much idea about laser cutting,its limitations,capabilties..So i find it difficult to think from manufacturing point of view..
but from images,i can see that it requires more metal,wastage of material is also more.thats we want to avoid.
David if I understand you correctly you plan to cut circles and then stretch them with hyd cylinders, if that is the case you will have issues as the flat pattern on flighting is not a true circle, because when you stretch the metal the id and od will get smaller, (in the cross section). You will not get the desired results, one reason is the flighting is twisted in a die and you would need to do it the same way to get equal results, however just pushing it won't twist it.... IMO
The way to develop this type of part is create a ID helix and an OD helix (3D Sketch) and then do a sheet metal loft and then flatten them to get your proper flat pattern, then when you stretch the material on to a pipe it will match perfectly.
To get the proper perspective or correct view after flattening, you need to select the flat surface and hit normal to view and hit space bar and add a new view, then you're ready to do the dxf export for the laser or plasma cutter.
Blue Lines are true circles that I developed the helix from and the model is shown in the flat, that would be how you cut your flight...
Helical sheet metal was an issue for a long time for us, we manufacture mixing machinery and often require flat patterns for helical blades. I finally found the following method;
Tutorial: How to model helix as sheet metal part? - GrabCAD
which has proved to work very accurately. We use a specialist manufacturer to incrementally press the helix from a flat profile, and have found our profiles to be within a millimetre or so of the flat shapes they have empirically developed over many years. We are making helical agitators with outside diameters ranging from 600 - 2500mm, for what it's worth.
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