How do I constrain this sketch so it scales automatically?

[ravindraw]

I've spent 2 days but can't seem to get this right. Please see the attached drawing. It is a pattern of vents on top of a enclosure. What I wish to achieve

1. Be able to stretch/shrink the pattern horizontally and have it scale.

2. Be able to change the hole dia and height of the vent ovals as required. e.g 3mm or 4mm or 5mm.

3. Once done I want to replicate that downwards and mirror it across on the other side.

4. Be able to change the dimensions of the enclosure and have the vents fit inside.

I've tried several things like dimensioning using parameters, using vertical/horizontal constraints etc. If I copy the pattern and paste it below one way or another I land up in a situation where either Fusion 360 hangs indefinitely if I set a constraint or dimension or the holes (circles) jump all over the place and so on.

My current thinking is to treat each row as separate and anchor it between 2 lines. So if the gap between the lines is increased/decreased the largest oval stretches across.

I understand..

a) There are smaller ovals and they would expand proportionately as their width would be set to be a % of the largest oval.

b) I may have to repeat the copy and mirror so as to only fit as many vents as possible depending on the total size of the enclosure.

Would really appreciate any help. Thanks!

[TheCADWhisperer]

1. Tie your sketch to the Origin for predictable behavior on Edit.

2. Pattern Features (not sketch elements).

3. Do you have an (easier) example  where you have used Parameters before?

(I would not think this would be a good example for your first attempt.)

[aliobidi]

Hi , 

first make a parameter then make a dimensions on all parametric sketch and give them  the parameter name I called it "x"  ..look at the pic 

when I change the expression it work good 

when you finish to give them all a parameter use "Rectangular Pattern " tool 

then you can change the expression .. look the pic 

[aliobidi]

and make more than a parameter like "X" "Z" ..etc  for what you want to link with the sketch 
here is your file

[ravindraw]

Uploading a parameterised file. See what happens to the oval in the 3rd row from below. It seems although the oval is enclosed (black border) its not an entity. The simplest way to do that seems to be to make the 3 points (the end points of the top and bottom line and the center of the arc) be constrained vertical on both ends of the oval. I've tried that too but it still misbehaves at some point (e.g when adding spacing between the rows).

@TheCADWhisperer, I have tied the sketch to origin. I've used the rectangular pattern but am not aware of the concept of features.

@aliobidi, I've tried exactly what you've suggested. But as you can see in my example, as we add dims and full constraints it starts misbehaving.

Clearly I'm doing something wrong.

[TheCADWhisperer]

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@ravindraw wrote:

…I've used the rectangular pattern but am not aware of the concept of features.

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Extrude is a feature.

Revolve is a feature.

Hole is a feature.

Fillet is a feature. (Not a sketch fillet though.)

Chamfer is a feature.

Sweep is a feature.

Loft is a feature….

When you pattern a sketch element Fusion has to calculate all of the sketch constraints (and interactions) of each patterned element.  This is computationally expensive.

Use simple sketches, constraints resolved once and done.  Then pattern features, bodies, or components.

In your example forget everything except the boundary and ONE slot.  
When you can predictably and robustly control that one Extruded slot feature, then you are ready to add the next feature.

If you can’t parametrically control a pattern of a single slot Extrude feature, well… post your try here…

[aliobidi]

this is not parameter concept 
you have to try something easier  

[ravindraw]

@TheCADWhisperer, understood features. The issue is the company that does laser cutting here wants a DXF file so I need the pattern in the sketch.

@aliobidi, can you elaborate? I didn't follow.

I was able to achieve almost everything. Let me know if there's a better way. I followed @TheCADWhisperer's tip and treated each row separately. i.e no constraints shared between them. As I wanted the elements to flex between 2 lines, within each row the first element was constrained to the 1st line and the last one to the 2nd line. One oval was set to "flex" i.e it's width wasn't defined. Used constraints for the rest. Here is the result.

[TheCADWhisperer]

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@ravindraw wrote:

@TheCADWhisperer, understood features. The issue is the company that does laser cutting here wants a DXF file so I need the pattern in the sketch.

No.

You create a simple parametric sketch.

Parametrically pattern features as I indicated.

Start a new sketch.

P for Project and select the face.

This will automatically create your complex sketch for you.

Right click on the sketch in the browser and Export to dxf.

Much easier to create.

Much more computationally efficient for Fusion to solve.

Much much easier to edit as needed.

[ravindraw]

@TheCADWhisperer, is this what you mean?

1. Created a simple parametric pattern. I tried but couldn't figure out why some of it is not fully constrained.

 

2. Used extrude to create the feature.

 

3. Used the pattern tool to make the pattern and mirror it.

4. Hit "P" and selected the top face to create a sketch.

 

[ravindraw]

I repeated the same steps today and landed up with this. It is fully blue and I can't see the sketch properly even in the Sketch mode. Appreciate any clue on what I'm doing wrong. If you look closely you can see the pattern but I'd expect it to look like how normal sketches look. If I flip the body and do the same from the other side then I get what I pasted in the previous post. Is it possible to get rid of the gray/blue fill and see it like a normal sketch?

Again, thanks in advance.

[TheCADWhisperer]

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@ravindraw wrote:

Appreciate any clue on what I'm doing wrong. If you look closely…

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Uhm, no *.f3d file Attached?

[ravindraw]

I thought the mistake I made would be obvious from the way the sketch looks. Anyway, here is an example. The sketch 8 does not look like Sketch 2.

[ravindraw]

Any ideas?

[davebYYPCU]

Nothing wrong that I can see, but this is what AD delivers as normal behaviour.

In the old days the profiles would have been surrounded by purple sketch articles, now we have to workaround it.

Hover over any profile and it will highlight, those lines and curves projected in will remain invisible, unless you edit sketch and consume those articles.

Those of us Laser / Plasma and Profile cutting -

To get a purple outline, you cancel the automatic projection in Preferences, and then Project the body Face into an empty sketch 9.  

Save Sketch 9 - sorry it was Sketch 8 as dxf and import it, strips all constraint and dimensions, just as useless.

Might help.....

[ravindraw]

@davebYYPCU thanks but I don't know what are projections and articles. Still a lot to learn. Let me try disabling projections as you suggested and see.

[davebYYPCU]

Sketch Articles, any / all the parts of your sketch, lines circles fillets whatever is in it.

Projections, manual or automatic, copies of existing data, bought into a sketch to use, usually purple, unless you break the link, but automatic projections are invisible until highlighted.

The sketch you complained / questioned about, was all blue with no visible lines, because you had the automatic projection option in Preferences turned on.  Automatic projections, only show Profiles, (blue shading) and not individual lines circles fillets dimensions constraints etc,

Rant - but they are there, just invisible. Makes sense to some people, - End Rant.

[TheCADWhisperer]

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@ravindraw wrote:

Let me try disabling projections as you suggested and see.

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Turn these off in Properties - I don't know any pros who leave these on.

Take control yourself and Project ONLY what you really want.

In this case, you in fact want everything - the entire face for dxf.

P for Project and select the Face (not edges) will get ALL of the edges of the Face for you into one sketch for Export to DXF.

(Funny thing is - I turned this so long ago that I couldn't even figure out how you got into your issue, I sort of remembered it from years ago.)