Drilling of a half-shere

3D Design Volume Model
1

Hello

After much research I still can't find my solution, will a kind soul be able to solve my problem?

Explanation:

I have: half a sphere, hollow, constant radius, wall thickness 95mm (visible lines are just dividing lines)

I want: to drill the wall with lots of small holes; and each axis of small hole having to be oriented towards the center of my sphere => normal drilling to the tangent plane.

I made a sketch on a plan and I want it to wrap around the face to then do the material removal (for the moment I'm testing the sketch is not finished and you have to imagine a circle at each line crossing...).

 

The 'Winding' function does not work; I think it's because it's not a closed cylinder.

The 'Projected Curve' does not allow the removal of material afterwards...

 

How to do it? PLEASE

Thank you for your help!

 

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2

Hello 

Try it out by converting your part to sheet metal. Make your sketch with all your little holes flat then do a removal of material and if I'm not mistaken, it's a normal removal....

 

2 Likes
3

Hello

Stupid question, why don't you go through the assistance for the drilling with a 3D sketch and then repetitions?

PS: I tested on a half sphere of 500 radius and 10000 5mm holes, it works well except that my PC took about 12 to 13 minutes to do it ...

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4

Hello

Thank you for your answers.

The sheet metal work I had also thought about it but I can't because in fact it's a welded construction and in addition what you can't see is that my construction shaft is 20km long and I can't redo everything. And 'convert it into sheet metal' he doesn't want.

 

I can't repeat either because the distribution of the holes is not uniform over the whole sphere.

I'm going to try the 3D sketch anyway.

 

5

See this communication thread

http://www.lynkoa.com/forum/solidworks/repetition-circulaire-trouspercages?page=1

@+

6

GT22:

Not adaptable to my case.

My goal is not to simplify my task by doing the minimum in my sketch. I'm going to have to place every hole anyway.

So repetition doesn't work.

 

There is really no one way to project the sketch, as if you were sticking a label on the sphere.

7

So, the beginning of hope:

The 3D sketch with assistance for drilling works well for orientation.

But for the position of the holes, how do I do with my cadrillage?

 

Thank you

8

Hello

Do you know the x, y and z coordinates of your holes? Or failing that, calculate them?

If you have this data, we can make a macro that will place these points and do the drillings.

Can't use the repetitions even when using the variations?

9

Why not do only a 10° section or other to find the right junction and repetition of the body afterwards?

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So to give an idea of the size of the operation: the sphere is 8910mm in radius and the holes are 60mm in diameter. Each portion of the sphere must contain about 6000 holes...

As input data I have this: the cadrillage with all the good dimensions in development (so flat).

And this in cup, which I did. The problem is that I have to constrain each point with the plane and the surface, so I have to make all the cutaways.

11

Good... FYI, I had the SW hotline.

My miracle solution is in the SW 2017 version where it is possible to wrap a sketch on a sphere (impossible until now).

So, the best way to do what I need today is the 3D sketch with assistance for the drilling, with a repetition. Even if it won't give the exact result, this is the solution I'm going to opt for.

Thank you all in any case.

12

How is this part made?

By rolling and then pushing back the material?

Are the holes drilled before or after forming?

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13

Hello, I'm coming....^^

 

Repetition in one area can't work?

 

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14

Otherwise, you still have the option of making a section of your sphere flat and putting your holes in it, then creating a stamping tool. You will carry out the stamping and then a repetition of your section.

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15

Hello

Did you know that it is possible to make holes with just a straight line? The scanning material removal function must be used. With a 3D sketch and circular repetition, this should be achievable.

16

My problem is not so much to be able to repeat the function but it's more about how I place my sketch. So I didn't specify but it's not design, it's modeling based on a plan. So it already exists in real life, so the fab is more my concern. I have to reproduce reality as accurately as possible.

 

So, for my solution...

I did: assistance for drilling with 3D sketching. I placed all the points of half a portion on the inner surface. I built plans using the grid, to be able to make the lines of points. And to finish I rated them one by one based on the cross-sectional view (photo in a previous post).

Then symmetry (in orange), then circular repetition.

Now it's been 3 hours that the pc has been grinding, yes yes really 3 hours.. and it's not over!

17

Depending on the number of repetitions and drillings, it is very possible that your PC rams and crashes

As soon as the test was carried out so make sure that your repetition is not too greedy

This is when a Xeon is preferable to an i7

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18

For the moment it is running, the memory is working so I think it really calculates. I may lose patience at some point, though.

Moving to SW 2016 will also be a big step. For the moment we are in 2013, it's not nice. We had internal performance tests to compare the versions (yes at the beginning the gearbox didn't want to evolve), there's no need to nitpick, SW 2016 is a big evolution in terms of managing large assemblies.

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19

I have finally finished my play! So it took me 5 days...

To sum up, I did:

- a body = a portion of the half-sphere

- a 3D sketch of a hundred points to place each hole. Each point being constrained with the surface, a plane and place with a dimension (FYI, sketch entity repetition does not work in 3D sketching). As a result, it makes me lines of dots. Symmetry on the portion itself.

- 'Circular repeat' of corp. 'Combining' bodies.

- 'Remove the face and fill in the discontinuities' to fill in the holes that were not supposed to be there (welding of the plates inside the sphere or welding line which must remain intact => can be seen clearly on the image).

Thank you all in any case for your help.

I will try to do this in stamped sheet metal when I use it.

Have a nice day!