Holes in curved sheet metal

[daniel.ea.kron]

Hi. I'm trying to make holes on a curved sheet metal surface. The holes need to be normal to the face of the sheet metal of course. The intention is to make threads in the holes after the sheet metal has been cut out for production and been bent. As one knows, it is not possible to use the unfold and fold command for curved surfaces that do not have a "normal" face. Therefor I have to use the "flat pattern" command before makin the drawing.

My design consist of 2 curved sheet metals that will be bolted together with countersunk screws. Ideally I think the best result will be achieved if it was possible to make an assembly of the 2 components and then drill into both sheet metals using the hole command, and thereafter make the threads in one of the sheet metals. Is that possible? Note: I have the hole pattern in a sketch (maybe I can project the sketch onto the sheet metal?) 🤷‍♂️

I attach an assembly of two sheet metals that I want to bolt together.

NOTE: The holes (pattern) are found in respective sketch for each part (sketch2). It is the same sketch in both parts. Maybe I can add a sketch in the assembly which I can use to cut both screens? 🤷‍♂️ 

Sincerely
Daniel  

[TrippyLighting]

Project the location points of the holes onto the curved front face of the red sheet metal part using the "Along vector" option

Then you can create a construction plane tangent at point. Then you can sketch circles onto that plane and extrude your holes.

[stiller.design]

Another way I usually do that is to "unfold" the sheet metal , then you cut out the hole as you normally do and at the end you refold the design again....et voila 🙂

@TrippyLighting solution works also 100%

[daniel.ea.kron]

Yupp. But unfold and fold does not work on curved surfaces that are created from a non-straight line.

[TrippyLighting]

If you use unfold - create cylindrical hole - refold, then hole will lose it's cylindrical shape with the refold.  

[daniel.ea.kron]

@TrippyLighting .True that (flat pattern holes become oval when folding). I'm thinking that it should be possible to extrude all holes with the surface tool and therafter intersect with the sheet metal. Wherafter I use the press-pull command on the "holes" faces to make them go? 

Update: i tried it and it works, but it is not possible to make threads on them. I guess the "holes" are not seen like holes? Maybe you know a way to make this work? 

Best regards

Daniel

[laughingcreek]

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@daniel.ea.kron wrote:

...i tried it and it works, but it is not possible to make threads on them. I guess the "holes" are not seen like holes? Maybe you know a way to make this work? 

...

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just like if you were to ben a sheet metal part when you extruded the holes from the flat plane of the sketch to the curved surface of the part you got ovals.  if you need them to be cylindrical so yo can put threads on them then go back to @TrippyLighting 's first suggestion.

[daniel.ea.kron]

@laughingcreek Hmm. Well I guess I have to do like that for every single hole then. It will for sure be time consuming. But if that is the way to go then I have to do it. It would be nice to be able to use the hole tool to cut a curved surface since to hole command seem to work towards the "normal" of the face.

NOTE: just using the hole command will not work when sketching on the normal plane created from the point on the curved face since it will start to cut at the exact position of the point which will is not the starting point of the face (I guess this can be fixed if I just create an offset face from the normal plane.

Do you think it will be possible to make a circular pattern on the hole command?


//Daniel

[Warmingup1953]

Can you add a flat extension to your Sheetmetal bodies to create a Flat Pattern ( and later edit out the extension from the .dxf)?

[stiller.design]

just like in real life , a bend sheet metal with threads wont work if you made the thread "unfolded"

you know what I mean @daniel.ea.kron ?

....better use a nut 😄

[stiller.design]

yes... with features selected

[daniel.ea.kron]

@stiller.design Yepp I know. i just want the threads in the unfolded view for siaplay when doing renderings. Also a want them in the drawing showing the "final result" so that the manufacturer can drill and thread the holes when it is bended/rolled. I have never done sheet metal before nor have I done any drawings, but I assume one needs a flat pattern and a "finish drawing" with instructions how to drill and make threads? 

This also leads me to another question which I'm looking into now:

Is it possible to cut 2 bent screens (2 screens in a sandwhich, where screen one is in front of another screen) with the hole/cut/extrude (sketch) normal to screen one (as described above)? 

//Daniel

[davebYYPCU]

Try Deboss - planar sketch with the correct pattern of circles, 

cut both plates in situ, and then add the thread to the inner plate.  

Countersink mentioned, then, lot more work, is a modelled hole body in a component, jointed to the face of the the plate, at the points Trippy showed in message 2, then Combine Cut those  Bodies, into the plates.

either, Might help.....

[daniel.ea.kron]

Wow, thats seem complicated, but maybe it is the way to go. I was thinking if I could just copy the plane and sketch from which I made the hole in the front plate and paste it to the component of the back plate and then extrude it from that sketch into the back plate . If I do like that I assume that the hole center will be the same of the front and back plate 🤷‍♂️

regarding the countersunk hole in the front plate. I was thinking that I can just use the chamfer comand to set the correct values? The only values I need is the depth and angle of the countersink, which is possible to have in the chamfer. What do you think about that?

//Daniel

[davebYYPCU]

You can’t chamfer, as it will be constant depth around the hole, unless you want to fudge - design dependent now,  

Example put a big hole in a smallish bar and chamfer it, (needs a Revolve Cut.)

I am thinking the quick way will be to copy / Joint the finished hole geometry,

(For common processes, Insert To Current Design) - those 4 holes, is place 2, then Combine Cut (is just 1 operation, no need to keep tools,) thread twice then vertical mirror the features.

Might help....

[daniel.ea.kron]

It is possible to make a chamfer in the program though. I'm not sure exactly what you mean, but when chamfering in the real life, it will be the same with a constant depth since the tool will not be able to chamfer diferent depths 🤷‍♂️ Or well, If one uses a laser cutter with changing focal length then maybe it is possible. But this will probably be made with a "normal" chafering tool or chamfer drill tool. Did I understand you correct? I know that I have to change the depth of the chamfer to a value higher than the k-value for the screw (Ref. ISO10642 fasteners). The chamferring (countersunk hole) will be made after the sheet metal has been bent.

//Daniel

[stiller.design]

yes thats possible

[stiller.design]

down the rabbit hole...LOL

[davebYYPCU]

After bending - drill and tap operations, OK, but Chamfer is not a countersink Cut, due to the bent curved face.  Chamfer does work on flat plates, Revolve cuts work on curved faces.

Make a 2 inch diameter bar, drill 2  - 1 inch holes across the bar.  Chamfer one, and Revolve Cut the countersink in the other.  You get distorted geometry from the chamfer, but in your case could be splitting hair.

However, if you know the fastener, Insert them and Combine cut is too easy.

Might help....

[daniel.ea.kron]

Ah, After I posted I realized that you actually described what I thought I was doing 😅 Ofc you are right here. I understand now what you meant with constant depth. My bad 🤦‍♂️. I see that a revolve cut could make it and also intersecting with the fastener (God idea). You don't know if it is possible to use the hole tool and change the starting position so that the drill (hole) will start drilling where the first interference with the bent sheet metal is? Now it will start in the center where i Put my plane.


//Daniel