Pattern cut using Loft

[flightyan]

Hello, I'm trying to make Pattern Cut using Loft. the upper surface has 100 rectangular hole with 5x5 and the bottom has also 100 rectangular hole with 3.2x3.2. the size of upper surface is 52x52 and the bottom is 44x44 with height of 40mm. When I tried to make through cut using Loft, one 5x5 hole to one 3.2x3.2  is possible but hole pattern to pattern is not possible, if anyone has good idea of making this easier, please share. thank you. 

-Jay-

[flightyan]

Here's the *.ipt file I tried to work.

[SBix26]

What version of Inventor are you using?

I don't know of an "easy button" solution to this, but at the very least you only need to do one quarter of the individual sweep/loft cuts; the rest can be created by mirroring the first quarter.

I'll see what I can do with it.

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Sam B
Inventor Pro 2020.0 | Windows 7 SP1
LinkedIn

[flightyan]

Hi Sam.

Thank you for your reply. I'm currently using Inventor Pro 2018. 

I just thought about kind of "distortion" function which can resize the size of particular surface freely and the adjacent faces as well. I think this function works well with 3DS MAX. Unfortunately I don't see any function like that from Inventor 2019.

[JDMather]

See Attached.

I left last corner for you to do.

The key when selecting a sketch with multiple profiles is - the first pick selects the sketch - the second pick selects the desired profile within the sketch.

[SBix26]

Here's one way to do it.  Instead of creating the holes, I created the grid between the holes, and did just a quarter of it with two mirror features to complete it.

Also, I centered both top and bottom grid patterns (required for the mirror to work properly); note that your bottom grid is not centered.

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Sam B
Inventor Pro 2020.0 | Windows 7 SP1
LinkedIn

[WHolzwarth]

Here's another method with sculpting. I wouldn't like to do more than these 100 cutouts

2018 IPT attached

And yes, it is visible, what happens with misalignment between the sketches, as mentioned by Sam.

[johnsonshiue · Accepted solution]

Hi! There might be other ways to do it. Here is a solution, not precise but kind of close. I used a Guide Rail Sweep to do it in one shot. Please take a look.

Many thanks!

[flightyan]

Hi Johnson. Thank you for your suggestion. It is kind of what I want to try.

[flightyan]

thank you for your reply. It seems what I've thought....problem is if the hole is not just 100pcs or the array is like 15x15 in this case the circular array can't be used. actually my actual modeling has 725 tiny holes..however your suggestion really helped me a lot.

[flightyan]

thank you Sam. I tried this and it worked well  under the condition that the number of the holes is not more than 100pcs and the array is a pair of even number like 10x10 or 6x6

[SBix26]

Similar technique can be used for any number of holes, but the creation time and processing time for 725 holes (29 x 25 pattern?) will be considerably longer. 

If possible, post your finished model when you have it done, or at least an image of it.

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Sam B
Inventor Pro 2020.0 | Windows 7 SP1
LinkedIn

[johnsonshiue]

Hi! You are more than welcome! This is a very interesting exercise. Actually, the Sweep can work the other way too (from bigger side to the smaller side). I notice that the dimension was specified only on the smaller side. So, I assume the other side does not need to be as accurate.

Loft is a powerful tool. It is more like Freeform. It can generate shape quickly. However, it is under-constrained. You don't have total control over the shape. In mechanical design, Loft should only be used when the shape is indeed under-defined, like transitioning from a square to a circle.

Sweep is a much more rigid tool. Its definition is clearly defined by a profile and a path (plus guide rail or surface). If you use the same geometry input in other CAD software, you will get the exact same shape.

Many thanks!

[SBix26]

@johnsonshiue I think in this case that Loft does give a precise and repeatable solution; all the faces are planar and edges are linear, which is exactly what one would expect.

@flightyan Here is another attempt, this time with:

• odd numbers of holes in each direction
• not square
• only two loft features plus two mirror features

showing that this can be extended to a variety of problems.  I will not volunteer to do it for 725 holes(!), but I think it can be done.

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Sam B
Inventor Pro 2020.0 | Windows 7 SP1
LinkedIn

[johnsonshiue]

Hi Sam,

Yes! Loft in this case does generate simplified faces but it comes with a cost. For Sweep, I only need one feature. For Loft in this case, I will need to create multiple features to get the precise shape. Certainly, Sweep in this case would not generate the exact shape as the two profiles (only one inside can be satisfied). But, I believe the design intent was having a tapered protrusion of a porous profile in a given distance. Otherwise, the other side of the profile has to be specifically dimensioned.

The more I know about 3D solid modeling, the more I think about how to make the shape in real world. 3D Printing can pretty much make anything. But, is the shape useful? Does it achieve the required tolerance? I personally think the current 3D Printing technology has room for improvement. At the moment, it is pretty much pixelated, essentially you place a drop of print material in the space layer by layer. Ideally, it should be more like the Brep geometry. The boundary should be clearly defined and then fill the internal void with lattice or solid. Sorry, I deviate the discussion!

Many thanks!

[SBix26]

No worries, the discussion is interesting!  I generally try to avoid lofting, but if there are actual dimensional requirements in this particular case, it seems like the only reasonable method (helical sheetmetal design is one other case).

For what it's worth, my last attachment has only two loft features, so it's not horrible.  But it means carefully constructing sketches; I've discovered that profiles that are easily selected for extrusion or sweep are not necessarily selectable for lofting, which is why it took two lofts to get the job done.

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Sam B
Inventor Pro 2020.0 | Windows 7 SP1
LinkedIn

[flightyan]

Hi Sam

As you mentioned, my problem was the fixed dimensional requirement, I made sketch for bottom side and used sweep with guide rail, not cutting. Of course it is hard to get the accurate size of upper rectangle, however by resizing the height and bottom, I could get closed number of what I originally want to have.

I'm going to 3D metal print with this drawing.

Thanks for everyone who helped me with this matter! 😆