Concentric circles, reducing inward

[onWXGDV]

I'm looking for a way to pattern a circle inside a circle, the diameter of the circle needs to get smaller as it gets closer to the center, is there a feature for this? the linear cutout, circular pattern would not work for my problem so I am stuck. 

@onWXGDV Your post has been moved to begin a new thread, and the title modified to improve findability by CGBenner.

[TheCADWhisperer]

@onWXGDV 

I don't know of a way to pattern that, but Thin Feature Extrude might cut your number of circles needed in half.

What are you attempting to model?

[jhackney1972]

You can use the Offset command, in your sketch, and repeat as needed changing the value as needed.  You must be sure to check the "Match Topology" box to be able to offset a previous offset circle.

[onWXGDV]

Trying to make a parametric file where the number of circular cuts can change, the problem I am having is when I pattern in the sketch the cut applies to the profiles I select however when I increase the quantity of the cutout profiles in the sketch it does not change the number of cuts. this is why I am trying to do it as a pattern feature instead of a sketch pattern. Basically I am modeling a big cylinder with multiple circular cutouts on the bottom starting at the edge and moving inward. There is no concentric pattern feature so Im guessing this isnt possible and I will have to settle with manually changing something every time I change the number of cutouts I want. 

[g-andresen]

Hi,

can you show a picture of such a real existing object?

günther

[Warmingup1953]

I am having difficulty visualising your problem. Can you post your file with further explanation and/or hand sketches if warranted? Is a "cutout" a circular hole?

[TheCADWhisperer]

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@onWXGDV wrote:

 I will have to settle with manually changing something every time I change the number of cutouts I want. 

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If there is any sort of pattern - it should be doable without manual editing.

[bergie5737]

Thank you, I am aware of it, but not an answer to my question as it is rather painfull. Basically, I'm looking for a concentric pattern. It will save me time, but for now, I had to do it the hard way as you described it. Ideally I want to make a body into a concentric pattern. 

[bergie5737]

I was trying to model something like this. Ideally a concentric pattern for bodies would be perfect. 

[davebYYPCU]

Doesn't have to be concentric pattern to do these.

Might help....

[TheCADWhisperer]

@bergie5737 

Your problem description title says "Circles", but your image shows Polygons (specifically hexagons).

Check back in a few minutes for a video demonstrating a general Pattern solution (that will work with circles or polygons).

[TheCADWhisperer]

@bergie5737 

See 1 Simple Sketch

See 1 Simple Thin Feature Extrude (could be of an arc rather than line).

I did the pattern as Bodies rather than as Features, you can change as needed depending on Design Intent.

I didn't Join the Bodies as I don't know where you are going with the Design Intent.  If I knew the Design Intent, I suspect it would be trivially easy to Join Features as they are created rather than having to Join Bodies manually.

Of course, if you want the center to be solid as in your image simply Extrude the interior triangular profile.

[johnsonshiue]

Hi! This is more like a progressive offset. You could use Sketch Offset or Surface Offset repeatedly to get the desirable geometry.

Many thanks!

[Warmingup1953]

Why not use a Rectangular Pattern driven by Parameters in Sketch and Revolve? 

Edit: Sorry let me do that correctly and post again!

[TheCADWhisperer]

@Warmingup1953 

Changes in Sketch Patterns do not automatically update in Features.

Try changing Number to 10 or better yet 100 and observe.

Hmm. my example doesn't update either.

Looks like I need the Pattern as one Body (Feature-Join).  After all, rings shouldn't be hanging in space.

Probably easy to do if I knew the Design Intent.

@onWXGDV 

Take this further and I will update my example so that it does automatically Update.

[Warmingup1953]

Yes, my Physics Lecturer back (almost) in the £sd days used to say "A great solution requires a very well denied problem!"

[bergie5737]

Hi, yes. It was circles, but as I was looking at re-creating that design and I uploaded it as an example.

I was 3D printing disks where I required a concentric "infill." It was very specific. If you know what a concentric infill looks like in a 3d print, you will have an idea where I am going with this. Just few weeks ago I had to design a stamp with concentric rings. The design was too complex to use the methods described, so I ended up using "offsets" in the sketch. In the end I discovered that a "concentric infill" in the slicer with no top surface almost worked, but a moment of clarity and a lucky discovery came up that the grid infill is perfect with the correct spacing. Thus I ended up with a "hollow" design and an infill that did the job.

I wonder how 3d print slicers generate a concentric infill as that sort of maths is beyond me!

[onWXGDV]

This is what I was doing however, when I update the number of rectangles I need to go into the revolve feature and reselect the new profiles. Not sure if there is a way around this. 

[KristianLaholm · Accepted solution]

Make the pattern the perimeter of the profile, if there is only one profile in the sketch Fusion will in most cases not loose track of it.

[onWXGDV]

Awesome this solves my problem perfectly! Thanks for the help.