How to Create a Sketch Driven Hole Pattern Normal to a Curved Suface

[Anonymous]

Hi,

I'm looking for some help creating a hole pattern that isn't a circular or rectangular pattern. I have about 200 points where I need holes, and I need the holes to be normal to the surface of the curved shape.

In the attached file I need to have the hole replicated on all of the points, with each hole normal to the curved surface. When I use the sketch driven pattern I can get the holes to follow the pattern, but I can't figure out how to get them normal to the outside surface of the shape.

I think this is probably a simple answer, but I haven't been able to figure it out after doing a lot of searching. 

Any help is very much appreciated

[CCarreiras]

Hi!

It's a simple answer... but not good... there's no way to do that, and the problem is, the holes have to be normal to the face.

With ths method is impossible, but there's other methods.

[Anonymous]

Thanks Carlos. What are the other methods that I might be able to use?

I really appreciate the help.

[CCarreiras]

How do you meant to produce that?

it's a sheet metal roll?

[Anonymous]

It will be 3D printed

[WHolzwarth]

Here's a way to go (2017 file)

Walter

[Anonymous]

Thanks Walter. I was able to get it to work like that, but now I'd like to take it a step further.

In reality the holes won't be following those original points because they need to be the same distance apart when following around the thread/spline.

What I did is I created a spine using the original points, then made a rectangular pattern of new points along that spine. On each of those points I need a hole that is normal to the surface of the curved shape. 

I can do it by creating a plane through a point normal to a curve on each point, then creating one sketch and copying it to the plane on each of the rest of the points. This is not ideal because it's repeating the same thing about 400 times, but it's a way to do it. 

The way I'm getting the holes cut right now is by clicking every single sketch and doing an extrude command. This is where it gets very time consuming because this takes a lot longer than copying the sketches, so my question is:

Is there a way to do one extrude command and select more than one sketch?

If there is, then I can click extrude, then go through and select every sketch and not have to open the extrude command ~400 times.

Thank you so much for the help on this! I really appreciate it.

[WHolzwarth]

Hmm. Good question. But it seems, that I'm out now.

Looks like task for Autodesk development. 2017 file attached.

Walter

[johnsonshiue]

Hi! Here is another approach. Basically, I create a double-circular pattern of workpoints. Place the part and a cylinder tool in an assembly. Use feature-based component pattern to pattern the cylinder tool. Lastly, derive the assembly (set the cylinder to cut) as the final part. Please let me know if you have any question.

Thanks!

[WHolzwarth]

That's not tricky enough, Johnson.

- No helical path around the basic shape

- No constant distance between holes

Thanks for your input. It's not the solution, but it's well appreciated.

Walter

[WHolzwarth]

Hmm. Hopefully Johnson is still watching.

I tried to place the bolt in the attachment with a sketch driven pattern. But I didn't succeed.

Is this normal?

[stuart_smith82]

Hi,

I might be missing something here but isn't the attached file what you are looking for? 

Thanks

Stuart Smith

[WHolzwarth]

No, Stuart. Equal distance between points along the curve is missing.

[Anonymous]

Hi Stuart,

The wording is a little confusing on this one, sorry. What I'm looking for is equal distance between the points along the spline/thread curve. The model you attached has equal distance vertically, but not along the spline/thread.

In the attached picture I need the distance between each hole (red dimension arrows) to be equal. The vertical distance doesn't matter.

I can achieve this by creating separate planes, sketches, and extrusions on every point, but to do that I need to create ~400 planes, 400 sketches, and 400 extrusions that are all identical.

I can copy and paste the sketches 400 times, which still isn't ideal, but only takes 3 or 4 minutes, so it's not a big issue. The issue is having to create a separate plane on each point and create a separate extrusion on each point. Creating those is where it gets extremely time consuming.

I know there's an option to copy and paste an extrusion, but after creating a first extrusion, I haven't been able to get the copy paste command to place the extrusion in the right place on the new planes.

Thanks again for the help everyone!

[Steven_Gao]

Hello,

I just tried your model and get the attached result. Please refer to the attached file to see is it your expected.

[WHolzwarth]

That's not the goal, Mingwei

Would you try Curved Shape Hole Pattern 2.1-WH.ipt ‏916 KB ?

Thanks

Walter

[Steven_Gao]

Hi Walter,

I took a closed look at your provided model. I saw you used 3D equation curve and Pattern with curve length to generate the work points. I tried to use sketch driven pattern to generate the pattern feature but I failed to locate the features on the normal direction of curved surface. It looks like the work points may not be on the curved surface accurately.

So I have to new a 3D sketch and use the Project to Surface command(Project to closest point), select the all work points(window selection) and project them to the outer curved surface, and then select all points and change their type to Center Point. Finally, I used the sketch driven pattern and generate the all cut features and they are normal to the curved surface.

But I also saw several points on the top and bottom are failed to project. Please refer to the attach model for details.

Hope this helps.

[Steven_Gao]

More edition of the part - I used the Project along vector to handle the failed project points on the top and bottom sides. Refer to the attached part for details.

[WHolzwarth]

Thanks a lot, Mingwei

I can see it done, but I can't reproduce it with my file.

Don't spend more time in it; I'll make a new attempt tomorrow.