Extrude a channel in a circle on different planes, with different diameter

[per.svanstrom]

I'm new to Fusion and I just love it. Trying to build a model for a CNC object and can't for my life find out how to create a specific detail in my Component. 
It should be a 360 cut with a growing diameter ending on a plane below the plane I started. Pretty much like a Coil with 1 turn, but I want different start diameter and end diameter. Trying to design a custom pump top for a water cooled scratch build PC. 
I'll add a link to a stock top, to show the angled cut out, its the inner swirl that ends at the outlet thread.

D5 Pump top image

I hope this is how I share my document. Thx in advance

http://a360.co/2pfOyFt

[mroek · Accepted solution]

You can use a coil to get a center rail guide, and then loft between two different size profiles at each end of the coil, like so:

I just created a new body here, but you could of course use the loft to cut out of another body, or use the combine tool afterwards.

This was just a generic example for you to look at, and I've attached the archive to this post so you can see it step by step.

[ian.q.young]

Hello 

I am a student of Fusion as well. 🙂

On YouTube there are a lot of Fusion 360 tutorial video's 

Here is a link to custom threads that may help.  The one that makes the thread in the plastic cap is close to what you describe.

link to tutorial vids

Hope this helps. 

[per.svanstrom]

This is great. Thank you so much. Can prob get this to work. But I can't replicate your file. 
I create a coil. I create 2 new construction planes (planes along path). Set one to 0 and the other to 1

Create 2 sketches. One on each plane.

Creates a loft and choose profile 1 and profile 2, but can't get a centerline

[mroek · Accepted solution]

What I did was to project the edge of the coil as a 3D curve (Project - Include 3D Geometry), and used that as a centerline for the loft.

[per.svanstrom]

Thank you very much, that was the missing link. Thx alot /bow

Will try to finish my model now 🙂

[per.svanstrom]

I'm appending to this thread instead of making a new as it's related

Now I manage to make my shape and everything execpt the final cut. I went about the same way. Created a new coil, created 2 planes, added sketches, 3D path etc, but I'm not allowed to cut.

Re-done the entire model from scratch, twize. Tried different sized of coil, sketches and nothing works. Same outcome everytime. 

Hope someone can help me figure this out. So close to a finished model and spend the entire day on it. Happy that I learnt so much about Fusion today (my 3rd day so far) but a little frustrated that I didn't manage to figure this out so far. Did a screencast to show the last part and the error message. 

[mroek]

It would be easier to help if you attached an archive of your design (*.f3d).  🙂

[per.svanstrom]

Ah, I appologise.

Here is a link, hope that works: http://a360.co/2pDLNuw

[mroek]

The link works, but exporting the archive to a file and then attaching to the forum post is more convenient for others, since it can then be downloaded directly.

Now, the issue you are having is something often referred to as "sliver geometry". Here's an image showing the main problem area (I did the loft as a new body instead of a cut):

I'm afraid this is because of inaccurate modelling techniques, so to fix it properly most likely requires a careful review of all you did, and also to know exactly what your intents are. However, a crude (and equally inaccurate) quick-fix is to press-pull the inner surface of the lofted body to make sure it overlaps the problem area, then combine cut. This will also remove material that you don't really want to, so it is not a proper fix. I've attached an archive that shows this method, but again, it isn't really a fix, more of a badly broken band-aid.  🙂

[per.svanstrom]

I'm not sure if I follow, but if something isn't up to CAD standard, I wouldn't be surprised 😄 My third day CADing ever. 
I actually wanted that small overlap, as I will add a hole from above to make a soft rounded end edge that starts from that overlap. So was my design intent. 

I need that to ensure proper water flows and deviding inlet from outlet. 

The idea is to create a custom pump top for a D5 PWM pump for water cooling PCs. I didn't want to do a one full coil as in the first example, as only the last 25% of the turn will need to be 45% downwards (if that makes sence)

I thought of this overlap and made a test with a shorter (less turned) coil to have 0 overlap, but got the same error message. 

PS. Thx for the input about the upload and your help. DS. 

[per.svanstrom]

Might be that I'm overcomplicating things. In an ideal senario this model should be millable in a CNC (Will that require something extra from the sketch, model I need to think about?)

Basically I just want to create different sized extrudes, last one with an angled base. "On" one of the inner circles I want to create a width-growing swirl from 0.1mm to 7mm during 280 degree swirl. Then in the last 80 degrees I want to keep the width continuing growing but decline in plane by 8mm. This is to create a swirl channel for pushing water to the outlet. 

At the outlet I want a 1/4 thread with the lower part of the 1/4 thread at the base of the 8mm lowered plane. If that makes sense. 

I have attached a very simple photoshop sketch just to show what I'm trying to create.

The red is the cutout

The green is where the growing diameter will stay level to the plane

Blue is where the drop in plane should happen

The red lower spline is just to show how the decline should behave. 

The outer white circle is 8mm higher then the red and the inner white circle is angled from the edge into the middle where it's 3mm lower in the center then the starting edge (that is levelled with the red)

It's obvious that my Fusion 360 skills isn't good enough yet, but quite happy with my progress after some hours in the CAD world, rather they days or weeks. I apologise if I add questions to this community at a to low level.

[per.svanstrom]

Realize how much errors I do when I create my sketches. Went through all the base tutorials today and manage to create first part of the model in a lot less steps. 

Would be very welcome to get feedback on the Fusion quality up to this step.

Now I'm lost on how to best go about to create that swirl decline cut explained in my above PSD post. Hope somone of you pro's have mercy on me and nudge me in the right direction 🙂

[mroek]

First, I wouldn't recommend using the hole feature for this. You have much better control if you create a profile sketch and use the revolve command to cut out the base shape of the main cutout.

I still have some issues understanding exacly how the spiral-shaped cutout should be. In your drawing you show it from the top view, so perhaps you should start with a sketch of that (the red) shape. For the spiral contour you can either approximate and eyeball it with a spline, or you could use the coil command to create a spiral (use the dropdown), and then project the edge of the spiral to a sketch. However, it is difficult to properly control the dimensions of this, since you want specific distances at specific angles.

The main issue is understanding how the depth of this cutout should be. Are you saying that the depth is constant for the first 280 degrees, and then you want it to gradually cut 8 mm deeper for the last 80 degrees?

[per.svanstrom]

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@mroek wrote:

First, I wouldn't recommend using the hole feature for this. You have much better control if you create a profile sketch and use the revolve command to cut out the base shape of the main cutout.

My reason for a fixed base and then holes (or could do sketches and extrude, not sure which are preferred tbh) is that I want to have a flexible base design, but the holes / cutouts are always constant as they are defined of the pump that will go in them. 

Realize that I could still just position the profile sketch on any base. Will change that!

I still have some issues understanding exacly how the spiral-shaped cutout should be. In your drawing you show it from the top view, so perhaps you should start with a sketch of that (the red) shape. For the spiral contour you can either approximate and eyeball it with a spline, or you could use the coil command to create a spiral (use the dropdown), and then project the edge of the spiral to a sketch. However, it is difficult to properly control the dimensions of this, since you want specific distances at specific angles.

The main issue is understanding how the depth of this cutout should be. Are you saying that the depth is constant for the first 280 degrees, and then you want it to gradually cut 8 mm deeper for the last 80 degrees?

Exactly this! Thats why I gave up on the coil command as that is a constant rather then gradually. 

I actually managed to make this cutout yesterday, but not sure if I did it correctly.

I did a sketch circle with the same diameter as the inner radius of the cut out. The did as with the coil and made 2 new sketch planes on path and placed them 280° apart and made a loft. Then I marked the end flat surface of that loft and extruded it with an angle. Then I made a circle sketch at the end of that extrude, but from top and extrude down in level with the extrude. It produced a cutout exactly as needed and without errors.

Not sure if it is the correct way to solve it though 🙂

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[mroek]

Good to hear! There is no such thing as a single correct way of modeling something. If you found a method that works, and produces the desired result, then look no further.

[per.svanstrom]

Not working. Almost about to give up. 20h in trying to make one cut, not funny anymore

Problem I run into with all my methods of creating the swirl, is that as soon as I change any dimension in my sketch, the entire thing breaks. I need to find a way to create the cut and tie it to my center point, so that if I change dimensions of the entire model, it follows. 

So frustrated right now...

[mroek]

If you have a model that shows what you are trying to achieve (albeit if it breaks when you change sketch dimensions), then you might get better help if you post an archive of that model to this thread.

[per.svanstrom]

I finally solved it, with a combination of sketch planes, loft, extrude and sweep

[mroek]

Good! Even if it was a long journey, you probably learnt a lot. 🙂