Creating rectangular pattern

[Anonymous]

I looked at here:

https://forums.autodesk.com/t5/design-validate-document/choosing-rectangular-pattern-plane/m-p/64746...

https://forums.autodesk.com/t5/design-validate-document/bug-sketch-rectangular-pattern/m-p/6374053#M...

And I did these steps:

1) Select editing plane by clicking on the plane in canvas.

2) In the Model workspace, select Create Pattern Rectangular Pattern.

3) Select the Pattern Type to set the type of object to pattern.

[Step 3 :  I select "pattern faces" from the dialog box,

then clicked "Select" for object for step 4 below. ]

4) Select the objects to pattern.

[ On the plane in step 1, I tried to select circle, but it does not select. 

I actually want to select 3 objects (using Ctrl + click objects),

but selecting one does not work.....  so I stopped! ]

Did I missed a step in screencast below?

 Thank you.

[jeff_strater]

Hi @Anonymous,

What are you trying to accomplish with your pattern?  Today, Fusion can either pattern bodies, components, or sketch entities (curves, points, lines, etc).  It looks like you might be trying to pattern an entire sketch?  That is not supported today.  If you edit the sketch, you can pattern the sketch entities (the circles).  Or, you can put the sketch into a component and pattern the component.

If you can provide some more details about your goal, there is certainly a way to achieve what you want to do in Fusion, and I or someone else will be happy to show you how to do it.

Jeff

[Anonymous]

Thanks @jeff_strater.

I am trying to pattern the left-most column of 3 circles.

Meaning I want it repeated a few more times on the left side of the left-most column of 3 circles.

But i cannot even select one, as you can see from the screencast.

Why is the circle not selectable?

And how to do I create a pattern of 3 circles?

[TrippyLighting]

In your screencast is seems you are trying to select a construction plane and pattern that. This cannot be done.

Then you attempt to select the circles in the sketch without being in sketch editing mode for patterning. That does not work either.

Then you select the patterning tool from the "Create->Pattern" menu, which is used for patterning 3D entities, not sketch objects.

1. To pattern the three circles you need to be in sketch editing mode.
   • In the browser, left-click to select the sketch that contains the circles, then right-click and select edit sketch.
   • You can also double-left-click on the sketch in the browser to enter sketch edit mode.
   • Usually in sketch edit mode you should be able to see the sketch pallete.
2. Once in sketch edit mode, select "Sketch->rectangular pattern". Select the 3 circles as objects and provide a line, construction line or axis as a direction etc.

[Anonymous]

@TrippyLighting:

Thank you.

Here is the screencast .

Note I did what you posted.

Still not able to select the circles.

Here is the public link of the file:

Fig C2 : Public Linked (Problem with selecting object in Sketch17 for rectangular pattern)

[TrippyLighting]

My suspicion is that you've not picked the sketch the circles are paced on.

Here it'll get a little repetitive. I believe on every single thread you've started and have  we've  asked you to please share your desing.

If you'd do that right with the first post, we'd be already done. So please.....

[Anonymous]

@jeff_strater

Just a note:

I have provided a public link here of the Fusion360 file to share
But when I clicked on it, it got to this link:
https://myhub.autodesk360.com/ue2927865/g/shares/SH7f1edQT22b515c761ef93d7b1ebd27e4cb

And I am not able to see it at the autodesk360 link.
Then Fusion360 crash and generate this report (this post) that I re-pasted here!

Auto web report response:

Thank you for sending your error report CER_135592459 to Autodesk.

We will analyze your report to determine how it can help us to improve our products and your experience with them.

 Addendum:

I think the uploaded F360 file it is available now....

[TrippyLighting]

I downloaded the file, opened it and am looking for a sketch with all these circles, but I can;t find it.

Is this the same file and version you are using in the screencast ?

[jeff_strater]

Hi @Anonymous,

The links you provided to point to a design, but not the one in this thread.  There is no sketch17 that I can see, and I don't see that pattern of circles anywhere.  Here is what I see in that design:

As @TrippyLighting says, you need to identify the sketch that those circles are a member of, edit that sketch, then you should be able to use Sketch Pattern to create a pattern of those circles.

Jeff

[Anonymous]

 @TrippyLighting:

That was an old file but I have no idea what it it.....

Here is the file:

http://a360.co/2cuqHww

Correction to folder name:

 See browser folder: Component2-FigC2:1 > Sketch17

Addendum:

If you can, show how.

I follow this step on dimensioning:

http://www.autodesk.com/products/fusion-360/learn-training-tutorials?utm_medium=product&utm_source=f...

Consider:  sketch Component2-FigC2:1 > Sketch-50mmProjectSShape

I tried to measure entire length from left arc to right arc.

but every time I click on the arc, it tries to measure the radius.

What I want is to measure left most point on left arc to right most point of right arc.

It should be about 300+ mm.

Basically I want to do a point to point measurement.

But it does not let me do so.

Thank you.

[Anonymous]

@jeff_strater:

I thought I uploaded the link correctly.

Anyway, I re-upload the link.  See my respond to @TrippyLighting below.

I did follow the steps to edit the sketch, but not able to

perform rectangular pattern operation on sketch circle(s).

So instead I select the circles by highlighting it.

then copy and paste.

Not what I desired, but it works.

[TrippyLighting]

It took me a while to figure to what might be the problem here, but there are so many issues with your design approach. At some point in time when you moved your sketch objects you moved them in Z-direction, instead of just in the X-Y direction  away from plane they were created on.

The is likely causing the problem. I am sure @jeff_strater can comment on this with more insight.

The little bit of geometry you've created so far could have been create with 2 sketches, 1 extrusion, one loft and a pattern for that one rectangular loft.

[Anonymous]

@TrippyLighting:

>> "At some point in time when you moved your sketch objects you moved them in Z-direction,

instead of just in the X-Y direction  away from plane they were created on."

Yes, I project the shape onto various construction planes in z-direction.

All those circles in sktech17 are all on one plane.

I edited and re-posted in previous reply to you, to see if you can do a length measurement.

of the shape in sketch Component2-FigC2:1 > Sketch-50mmProjectSShape .

Thank you.

[TrippyLighting]

I think you are misunderstanding what I was trying to say. I hope this screencast explains that better.

[Anonymous]

@TrippyLighting:

Thank you.

Yes, I understood what you meant.

I am saying those circles in sktech17 are all on same plane.

I may have deleted the the construction plane after I projected the circles from sketch16

or I created the construction plane for sketch17, and drew those circles.

It is also possible I messed up and some of those circle sketch objects are not on same plane.

But I think those circles in sketch17 were also generated from rectangular pattern

While we are at this topic, I wonder if there is a tool to test 

if sketch objects are all on the same plane. 

It would be a nice tool to have.

I thank you for your generous time.

[jeff_strater]

as usual, @TrippyLighting has figured out the problem.  Yes, those circles are all on the same plane as each other, but they are not on the sketch plane of that sketch.  Sketch pattern only works on 2D sketch items that lie in the sketch plane.

There is no tool today to say whether a sketch object is on the sketch plane.  That's a pretty good idea, though.  However, there is a command that will fix the problem:  you can select geometry and use "Move to Sketch Plane" to force them to be in the sketch plane.  Then, you can create the pattern you are trying to create.

Here is a screencast showing how to do that with your design.

Sorry it took us so long to figure out the problem.  Once you were able to supply the design, it simplified the debugging process!

Jeff

[Anonymous]

@jeff_strater:

Thank you.

Great, the "Move to Sketch plane" will move to the edit plane where the sketch object is selected!