UN-EQUAL CIRCULAR PATTERN

[Anonymous]

Guys,

Any idea how to pull this off without manually doing it? I've attached an example of a 4 instance circular pattern, currently evenly spaced. I'd like to be able to pattern at an un-equal spacing, and can do it manually by creating individual patterns of the first memeber, but it is a long process for more complex parts. Any ideas?  How about developers who have coded something like this?

Thanks,

Rob

[mcgyvr]

Inventor 2017 can do it..New functionality there as far as patterning goes.. sketch based patterns,etc...

https://knowledge.autodesk.com/community/screencast/da14dded-ad0d-4ff9-a331-eea508e93721

You can also suppress instances of a pattern..

Maybe you can use ifeatures or the punch tool to place features on sketch points..

There is also curve driven patterns..

http://blogs.rand.com/files/curve-driven-patterns.pdf

More than likely you will need to manually do it though depending on the desired patterns if you don't have 2017..

[Anonymous]

Mcgyvr,

Thanks for the tips. We'll have to give sketch patterns a try after we install 2017.

Thanks!

[WHolzwarth]

Hmm. I thought similar as mcgyvr, that it could be a task for a Sketch Driven Pattern in 2017, but I couldn't get it.

Perhaps someone from Autodesk can tell, if it's possible.

Walter

[Anonymous]

Although I haven't tried the sketh pattern yet, I think it will still have it's shortcomings.

For example;

Take a bolt circle with unequally spaced clearance holes. You would probably still have to draw the bolt circle, radial lines, end points at the ends of the lines all before creating the sketch based pattern of the first hole.

You could achieve the same result by creating a single hole and doing multiple circular patterns of it at the different rotational positions.

The real quiestion is which is more work..

[SteveMDennis]

Sketch driven pattern is in 2017, it simply puts occurrences of of the features, etc. at the locations of sketch points from a sketch you specify.

It does not matter where those sketch points are we simply compute the features to be patterned at those points.

[WHolzwarth]

Hmm, Steve.

Can you show the solution for Rob's problem?

Thanks

Walter

[SteveMDennis]

Sure, hopefully a picture is worth a 1000 words. I turned the sketch on that is driving the pattern so you can see I just randomly placed some sketch points

[Curtis_Waguespack]

---

@Anonymous wrote:

Although I haven't tried the sketh pattern yet, I think it will still have it's shortcomings.

---

Hi ROBTRONIX ,

I think 2017's sketched patterns will be very powerful, but I agree that for an un-equal circular pattern it provides no benefit over anything we had in Inventor 2016 or before... unless I'm missing something.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

Guys,

Got to trying 2017 this afternoon. It seems to behave great for patterning multiple instances from base point to other points, but the orientation to the original remains in tact and does not seem to allow it to pattern while remaining circular. Is this correct?

Rob

[SteveMDennis]

Rob,

 I'm not sure exactly what you are asking... you have some control over the base point (I was doing holes so orientation to the original is constant).

"Does not seem to allow it to pattern while remaining circular?"

It patterns where ever the points are in teh sketch. If you put the points in a circle your sketch driven pattern will be circular.

I think you do need to try it and if you find a deficiency please let us know.

We just follow the points!

[Anonymous]

Steve,

I've attached an example of current workflow "manual" to create unequaly spaced circular patterns. You'll see an attempt at doing this by sketch based in the bottom of the document. Any suggestion would be greatly appreciated!

Thanks,

Rob

[SteveMDennis]

Rob,

  I see what you are saying now... and maybe this will not work for you because the sketch driven pattern does not have an axis so how can we rotate?

We also added the ability to NOT rotate in a circular pattern in 2017 but sketch driven pattern was done by another team so I am not as familiar but if we think about it w/o a center axis we can't rotate.

In the help it says:

Optionally, do the following:

• Select Base Point and then pick a new reference point to use as the pattern Base Point.
• Select Faces and then pick a face to specify the face normal direction for the pattern.

So I was thinking those controls did contribute to orientation but as much as I try I can't get the faces option to change my pattern at all!! Even if I pick an outer cylindrical face on my base...

I need to ask someone what the faces control is supposed to do.

Sorry that this may not do what you want/need after all but let me float out a question to the team that did this and see.

[SteveMDennis]

Alright Rob I found an internal video that shows me how it works... not sure I like it but you should be able to get there from here without waiting for my China team to wake up!!

So that cutout is irregularly spaced and rotated using sketch driven pattern!. It's not perfect because my points were not exacly in the center of my rim of my disk.

Keep in mind "I'm a software engineer Jim not a **** designer!" 🙂 (Star Trek anyone?)

What you have to do is use a 3D sketch around the outside rim of your part. Put the sketch points in the 3D sketch around the outer rim of your part, then you need to choose a base point that matches up with those points and for the face pick the outer cylindrical face that the points are on and it will use the normal of the cylindrical face at that base point to rotate your features being patterned.

Not sure if you will have the play with the optimized/identical options at the bottom of the dialog under the >> or not...

Yours is way more complicated than mine but you may be able to get there... hope this helps I just learned a lot about sketch driven pattern!

The face option in the dialog only makes sense when your points are on faces that are all not in the same plane.

[WHolzwarth]

That's interesting, Steve.

Now I'm eagerly waiting for the file.

[SteveMDennis]

Well I'm going to have to leave it as an exercise for the reader. I did do it using the OP file but I mistakenly did it in an internal early 2018 build which means it's useless to you guys! Sorry I was doing 2018 work and fired that version up by mistake.

Here is a picture of the original file with a single sketch driven pattern with the feature at 45 degrees, 85 from that, then 135 degrees from that.

[Anonymous]

Steve,

Thanks for the followup. I'm not exactly understanding how you've created the geometry in the last image. Could you possibly screen shot the underlying sketches needed?

Thanks,

Rob

btw your answering the prayers of many tooling guys!

[SteveMDennis]

I'll get one of our QA guys to do it and republish the file. I don't have 2017 installed right now...

Have to be Monday. 

But here is how the sketch is created for the above picture:

1. Create a sketch on the end of the cylinder
2. Project the circular edge (won't be full because of the cutout)
3. Draw some lines from the center to the rim (projected curve from #2)
4. Dimenions between the lines to create your different spacing (mine was 45, 85, 135 between each "spoke" line)
5. Place points where those lines meet the projected edge.
6. Now you can edit hte dims to your hearts content and the points will go along for the ride.
7. Create a sketch driven pattern
8. Pick the sketch
9. Pick the extrusion cut to pattern
10. Pick a base point that matches up with the points
11. For the reference Face, pick the cylindrical face that the points are now on (they are on the edge of the cyl face)
12. At those points the cylindrical face normal will be used to rotate the extrusion geometry at the base point

Voila! Should work.

[Anonymous]

Steve,

Got it to work, but had some trouble on step #11. I could not get it to select the solid model as the reference face. I had to create a surface model cylinder instead and it worked fine. I'll experiment a little this weekend.

Thanks for your help!

[AngeloGuo]

Hi Rob,

By using sketch driven pattern, you can get the expected result with different distance in your sample.

Here is the detailed work flow,

1. Create a 2d sketch based on the top of the cylinder

2. Project the edge to sketch

3. Creat sketch point on the circle(with distance you want）

4. Finish sketch

5. Start sketch driven pattern

6. Select sketch points, base point(should be on the reference face) and reference face as below picture

7. Click OK, then you will get the result

Please refer to the attached part file for more information.

Let me know if you have any problem with it.

-Angelo