Gap between sketch and curved surface

[yhaPM8SB]

Hello, i am facing a problem with creating/projecting a sketch on curved surface.
i am trying to create a hole surface projected to a solid cylinder, I use 3d sketch to use the project to surface feature but when i do that and try to zoom in i always see gap between the hole surface and the cylinder surface, i tried to create another cylinder solid body and use cut command between these two bodies but again i see always a gap between them.
I tried to use stitch as well, but no use it is not working, i also tried in fusion360 and same problem, and this gap issue should be solved so i be able make CFD.
any solutions or ideas ?

[YannickEnrico]

Depending on how far you zoom in, you'll always be able to produce a view where it *seems* like there is a gap.

Can you attach the part exhibiting the behaviour so we can inspect`?

[yhaPM8SB]

Hi, here  are two versions one with gap and one without.
problem with the way i did to fix the gap issue that it takes too many steps i want some faster way to do it

[YannickEnrico · Accepted solution]

Well, as I said, the software sometimes produces views where it seems like it doesn't touch - Usually provoked by excessive zooming in.

You'll have to trust that when you constrain something to a surface, it stays on the surface.

That being said, I'll attach two examples that produce a result that may be more to your liking.

[johnsonshiue · Accepted solution]

Hi! Boundary Patch isn't very precise. A tiny gap might be expected. Instead of using BP, you should use Split command and select the 2D sketch to split the cylinder. Then use Delete Face to remove the small circular face. Is this what you were looking for?

Many thanks!

[yhaPM8SB]

Hi, i come back with another question.
Actually the split trick is perfect but i have problem with pattern.
so if i have sketch which include 500 circle in pattern when i finish sketch and try to split the all of these circles, I find out that i am allowed to select only one circle for splitting and i will need to create new split manually one by one for each circle in the sketch.
i also tried to rectangular pattern the split feature itself but it didn't work as well.
is there any solution to split many circles from a face without gaps in quick way than selecting these 500 circles one by one. 

[YannickEnrico]

Maybe this approach works for you?

[yhaPM8SB]

Hi, thanks for your answer unfortunately it is not that case.

I want to have full solid cylinder with pattern of holes and these holes are just face on the cylinder without having any gaps.

in the last answer from Jhon he mentioned a trick to draw a circle and then split from the cylinder and then i will have a face without gap around the cylinder

and it is really helpful, the only problem it is not valid for many multiple circles. as in Split i need to select one tool and i can't select multiple tools. 

[YannickEnrico]

If I understand you correctly, this might work for you

[yhaPM8SB]

I see after the extrusion, if i zoom in i can see a gap and this gap make CFD fails.

in the part file i attached below you will find an example using a split command to split the circle from the cylinder surface without any gaps but the problem that i can't pattern this split

[YannickEnrico]

Have you tried CFD on my part? Because it's produced the way Johnson suggests, albeit with some patterning and deletion of different faces

[yhaPM8SB]

Hi, yes i tried the geometry isn't water-tight and i got error.

[YannickEnrico]

Yeah it's definitely not optimal that you can't pattern the split.

If you can make one layer on a slice of the cylinder, you can pattern the solid like I did in this attached example

[yhaPM8SB]

I understood what you mean, but this will only be valid if i have symmetric pattern of holes.
In my case i have multiple hole sizes and different placement of holes and also distance between holes are different from one hole size to another.
that mean i will not be able to make rectangular pattern for a slice of the cylinder. and get the pattern i want.
the split feature is really solving the gap issue but for pattern i am stuck. 

and one more thing, quantity of each hole size is different if i make slice and rectangular pattern, then all hole sizes will have same quantity as rectangular pattern quantity 

[YannickEnrico]

If you can find any kind of pattern in parts of it, you can use sketch driven pattern to pattern the slices differently.

Edit:

In that case you will have to model the slices as different solids, pattern them, and then combine all of them.

[yhaPM8SB]

i am a little bit confuse and i am worried that this also not working.
this the final part i want to have, could you please do it at your end with your method and try to get the same part with my required pattern

[YannickEnrico]

See this.

[yhaPM8SB]

yes I agree you managed to do it, but tbh it is so complicated and time consuming because i build similar cylinders every day too many times .
I really appreciate your time and effort but we need to find a more simple and faster way to do it.
I am trying to squeeze my mind to find a simpler way 

[YannickEnrico]

How do you expect to find a simpler way when it consists of so many different patterns?

[yhaPM8SB]

I do see that your way is valid for cfd, no gaps and all is fine.
but for CFD preparing the geo is just the first step, and and i will have many different cases of cylinders with elbow with different hole sizes and placement
and although the way you showed is really good for cfd but it will take ages if i do this for each cylinder i have.
i am trying to find a quicker way to use split with multi sketch without selecting it manually one by one.
when i do split for one circle and try to select it in rectangular pattern it looks like inventor doesn't recognize the split as separate face.
I am really lost and i want to find the quickest and efficient way to do it