Trying to create holes through a curved surface

[steve_hammonds2020]

Hello. I am working on a part that has a curved surface. The curve was created using a parabolic equation. I cannot simply select the face I want to create a hole through and create a sketch on it, I'm guessing that's because it's not a flat surface. I recently got help on here and was able to create a slot through the surface (here is the thread: https://forums.autodesk.com/t5/inventor-forum/creating-a-slot-through-a-part-along-a-curved-surface/... ). I was initially pretty satisfied with the result, but I later wanted to add some holes periodically though the surface so that you could insert cables and suspend the part from a ceiling. Anyways, I have yet to be successful at adding the holes, and on top of that I noticed a problem with the method suggested to create these features. When projecting the geometry from the 2d sketch down onto the surface of the part, the sketch becomes skewed due to the curvature of the part. This is most noticeable when viewing the holes at the bottom of the part because that is where the part is curved the most. I think that the holes will be fine because they are circular when viewed directly from above and as long as the hole is made cylindrical straight down from above it will be perfect for the cable to pass through. The slot, however, is also skewed due to projecting it down onto the curved surface. Again, it is most noticeable at the bottom of the slot. I would like to make sure that the ends of the slot have a matching radius. Additionally upon further inspection, I noticed that the slot was made normal to the surface of the part, which may be OK for the slot, even though I would like to know how to change the angle on which it is created if it ever needs to be changed in the future. This would not be OK, however, for the holes because as mentioned above, the cables will be coming straight down vertically through the part. So, how can I add the holes to this part AND ensure that they are created straight down through the part, possibly alter the slot to do the same, and change the profile of the slot so that the top and bottom have the same radius?

[pcrawley]

There's a bit to unpack in that question - but I think you are looking to cut the slot & holes normal to the parabolic curved track.  Is that correct?

My method for that sort of work is to flatten it - cut the features - and re-bend it.  In the attached, I added a short straight extrusion to one end (to give the "Unfold" tool something to hang on to) - converted it to sheet metal - Unfold - cut the features - refold - and finally delete the flat extrusion.

You may need to adjust the 2d sketch for the slot and holes because it is drawn for projecting vertically down onto the curved surface - not the flattened part.

Inventor 2024 model attached.

[steve_hammonds2020]

Hi pcrawley, I really like what you were able to do and in such a short period of time. In regard to the holes, I do not want them to be tangent to the surface of the part, but rather strictly vertical. Nevertheless, I appreciate you showing me this approach and I will do my best to unpack it all and decide if it is a viable method to achieve the result I am looking for.

[pcrawley]

Glad you liked it.  For the holes - when you say "vertical", do you mean they have the correct orientation in my model, but you don't want them 'squashed' by the refold feature?

I'm sure there are other methods, but I would use the Cut feature to add two small holes, then create an axis through the hole.  (There's a Workpoint creation option called "Center Point of Loop Edges" which I used to create the points - the axis passes through the two points for each hole).  Now you can use the Hole feature to cut the hole by selecting one Workpoint as the start, the Axis for the direction, and make sure you tick "Extend Start (under Advanced Options) or there will be a bit of the bent part left at the start of the hole.

[SBix26]

If all of these slots and holes are meant for suspending the track from overhead, then the simple solution is to simply extrude from a horizontal sketch all the way through the part.  Since this is so simple and obvious, I assume that I have not properly understood the problem!

Here is a section view through the part after extruding the slot vertically and placing the six holes vertically (arrows):

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Sam B

Inventor Pro 2024 | Windows 10 Home 22H2

[kacper.suchomski · Accepted solution]

You can make holes both by extrusion and with a hole tool.

[kacper.suchomski]

And this way you can properly model the gap, along with the possible tilt of the face.

[steve_hammonds2020]

Hi again pcrawley, sorry for the confusion LOL. I don't think your model has the correct orientation that I am looking for. The holes that are shown in your model are perpendicular to the surface of the part face. I think the best way to describe the desired result is to just say that the holes must be parallel to the Y-Axis.

[steve_hammonds2020]

Hi SBix26, I think that the section view you have provided shows what I am trying to accomplish, although I can't be too sure because a section view does not provide the same level of clarity that a 3D model would. And yes, this does seem like a very simple and obvious task, but believe me it was giving me a whole lot of frustration the other day. I am a beginner and I am pretty much teaching myself in my spare time. Thanks.

[SBix26]

OK, here is your file with the slot and holes as I described in my previous message (Inventor 2024 format).

Note that I edited your Slot Profile sketch and changed the hole centers to Center Points so that the Hole tool would find them all automatically.

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Sam B

Inventor Pro 2024 | Windows 10 Home 22H2