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Seven Pointed Star 241214

17 REPLIES 17
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Message 1 of 18
pittsallen
600 Views, 17 Replies

Seven Pointed Star 241214

Hello Fusion forum,

Working on a seven pointed star.

For several years electrical fixtures have been
designed and printed using Extrude and Revolve.

It is conjectured that the best way to
make the star is with Sheet Metal.
But this is my first sheet metal
part so some adult supervision is
elicited.

Have studied several tutorials like
https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-B98BC5F5-E640-40F6-B71D-151EDFE9586D
and several YouTube videos. None of them
apply to what I am trying to do. And I am
not sure what I am trying to do can
be done in Fusion.

On the Sheet Metal tab a Sketch of the flat
plate is completed.
seven_pointed_star_241214_b.jpg

With the flat plate sketched, the plate
should be folded against the centerline on the star
points so that the radii inside the construction
circle would come together.

If that can be done using the Fusion environment
could that part then be made into a Component that
could be 3D printed? (As opposed to actually
creating a sheet metal part with shear and
break machines?

Thanks.

 

Allen pitts

17 REPLIES 17
Message 2 of 18
laughingcreek
in reply to: pittsallen

I can think of a few dozen things you might mean.  can you hand draw a sketch of what you're trying to end up with?  

Message 3 of 18
g-andresen
in reply to: pittsallen

Hi,

please show a picture of a real existing object

 

günther

Message 4 of 18
pittsallen
in reply to: pittsallen

Hello @laughingcreek@g-andresen  and the Fusion forum,

Don't have a photo because it is an idea
similar to a star seen on top of a Christmas tree a couple of weeks ago.
But here is a rough sketch.
seven_pointed_star_241214_drawing.jpg
Thanks.

 

Allen Pitts

Message 5 of 18
Warmingup1953
in reply to: pittsallen

Do you simply want to model a 7 Pointed star like this:

Capture.PNG

 

Or do you want to create as a Sheetmetal project? There are some online origami patterns ...and I Guess paper could be seen as just very thin sheet(metal)?

 

 

Capture2.PNG

 

 

Message 6 of 18
TrippyLighting
in reply to: pittsallen

I would first work on fully dimensioning and constraining sketches, before moving to more elaborate techniques!


EESignature

Message 7 of 18
metalmasterscm
in reply to: pittsallen

Is the bend line ONLY through the centerline of each point?

 

Message 8 of 18
laughingcreek
in reply to: pittsallen

you see five pointed stars like this all over texas-

laughingcreek_0-1734236147734.png

 

 

unclear on what your end goal is.  do you want to end up with a Sheetmetal design, or just something you can 3d print?

 

attached is a model of an easy way to model a printable design.  and a vid showing changes to parameters-

 

 

Message 9 of 18
johnsonshiue
in reply to: pittsallen

Hi Allen,

 

Is this what you are looking for? All you need is a vertical sketch line defining the Loft vertex. Then create  the Loft by selecting the 4-sided profile and the point. Lastly, pattern it 7 times circularly.

 

johnsonshiue_0-1734369734895.png

Many thanks!

 

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 10 of 18
pittsallen
in reply to: pittsallen

Hello Warmingup1953, @trippLighting, @laughingcreek, @johnson.shiue
and the Fusion forum,

Warmingup1953
The image of the light blue seven pointed star is exactly
what the design vision perceives for the face of the star.

trippLighting
I would first work on fully dimensioning and constraining sketches,
before moving to more elaborate techniques!
The suggestion is valid and appreciated. Is it possible to
be more specific? How is a sketch 'fully dimensioned'.
How is a sketch fully constrained? Quite often when constraints
are applied an error message is returned saying the sketch
is over constrained.

laughingcreek
The metal five point star with the circle intersecting
the five points shown in the photo is also very similar to the intent.
I am from Dallas and have also seen these metal
stars in travels through the Lone Star State.
The metal five point star with the circle intersecting
has an aspect which is sought: the shape, because it
is made of sheet metal, is open behide the face. It is
not sure if Warmingup1953's light blue seven pointed star
is sold or hollow. The design intent is for the star
to be hollow so LEDs could be incorporated thru the face
of the model.

The excellent video has been watched carefully a dozen
times but I am not sure how it got started, what environment
the actions are being done or exactly what is happening.

The star.f3d is very helpful. The star.f3d is exactly
where I was headed. Is it possible for me to know how
star.f3d was begun and developed? A tutorial or a step-
by-step is not requested. But perhaps just a general
idea of how star.f3d was conceptualized, begun,
and developed.

After stumbling around for hours with the Sheet Metal
tab a return was made to my old friend the 'Solid' tab.

A sketch of triangle was created and extruded 1.6 mm
thick. Then the mirror image of the first triangle
was Sketched and Extruded.
Triangles_sketch.jpg
Then the two triangular Bodies
were rotated fifteen degrees from XZ plane and brought
together to create a Point Body.
Star post 241216_01.jpg

(Unfortunately a mistake was made in calculating the
angles for the triangle sketches so I ended up with
a six point instead of a seven point star. If another,
better method of making the model is not found
I will go back and decrease the angle between the
two sides of the point Bodies to make enough room
for a seventh point.)
Star post 241216_02.jpg

The process that was struggled with mightily was
aligning the the point Bodies. The Move command
is a sledge hammer where a scalpel is needed.
Star post 241216_03.jpg
I also tried Modify > Align and Assemble >
Joint. Perhaps the Assemble > Joint approach did not work
because I think Assemble > Jointis meant to be
employed with Components, not Bodies.

Thanks.

Allen Pitts

Message 11 of 18
laughingcreek
in reply to: pittsallen

in no particular order-

 

whether you chose to use fully constrained sketches or not, understanding the concept of what one is and how to achieve it is extremely important if you want to make models with out struggling to much.  an absolute necessity if you want to them to be fully parametric (such as the one I posted for you).   I suggest you put a lot of focus on this concept to make life a bit easier moving forward.  (side note: the "over constrained" error message you get happens when you apply a constraint or dimension that conflicts with a constraint or dimension that has already been applied.  example- if you try to put an angle dimension on a line that already has a horizontal constraint applied, you will get the "over constrained" error.)

 

I'm going to infer from your latest reply that you don't need a sheet metal model, but one that is hollow on the back side.  in this case the sheet metal tools are definitely NOT the way to go, but you seem to have figured this out already.  getting a hollow model from the model I posted will require one additional command tacked on to the end, so lets not get hung up on  that.  we'll do it next.

 

the video I posted shows me parametrically changing the file I posted for  you.  they are meant to be studied together.  Have you gone thru the timeline of my file?  open up and edit each item and study the settings and selections, see if you can suss out what's happening. (another side note: studying other peoples models have led to some of the biggest aha moments for me.  here on this forum you have the model author available to you for questions.  when ever someone posts a model for you take advantage of it).

 

in the video, at 14sec I am adjusting a user parameter that controls the number of star points.  (this only works because of the fully constrained sketches.)  lets skip this and go to the 34sec mark.  here I am adjusting 2 dimensions that control the over all size of the star. (the points and valleys.)  these are found in sketch 1.

right after I show changing the dimension that controls the height of the center of the star.  this dimension is in sketch 2.  sketch 1 and sketch 2 are used together as inputs for the next command (loft).  I'm going to stop here.  study these 2 sketches. ask questions. 

 

one thing to note about them is that they are fully constrained.  you can tell because they both have a lock glyph on them (yes, the lock symbol is confusing. doesn't mean its "locked", just that it is fully constrained)-

laughingcreek_0-1734394369608.png

when comparing my model and your model, you might also note how much simpler mine is compared to yours-

my timeline-

laughingcreek_1-1734394511229.png

your timeline-

laughingcreek_2-1734394528495.png

 

your timeline has moves, position captures, and base features.  IMO a well constructed model of these type shouldn't have any of these things.

 

something to think about.  if a hypothetical "boss" where to ask for you to make changes, such as to the overall diameter, thickness, height, or number of points, which of these models do you think would be easier to make changes to?

 

 

 

Message 12 of 18
TrippyLighting
in reply to: pittsallen

See the screencast:

 


EESignature

Message 13 of 18
pittsallen
in reply to: pittsallen

Hello @laughingcreek @TrippyLighting and the Fusion forum,

laughingcreek
Have studied the videos. It can seen how making
changes at Modify > Change Parameters alters the
models although how to set up Parameters for
a Sketch is still a work in progress.

The datum on the lock glyph is edifying.
Because there are some specific questions on
dimensioning and constraining Sketches a
separate post titled 'Fully Define and
Constrain Sketches 241217' will be posted
soon after this reply is made to separate
the subject of this post, the star, from
a specific query about dimensioning and
constraining Sketches.

 

The timeline of star.f3d has been studied and
some knowledge of the Create > Loft command
is being gathered.

 

trippylighting
Shout out to trippylighting for the excellent video.

Yes, the intent is to print the whole star.
And when the star shape is complete add
eight mm circles at the tips of the star
points with 5 mm holes in the circles at
the tips. Five mmm LEDs will go in the
holes. That is why the star is hollow
instead of solid because that will allow
a place for printed circuit board (PCB), battery and
wiring.

In studying the videos by laughingcreek
and trippylighting on my 15" PC screen
it is almost impossible to read the
dialogue boxes. Would it be possible for the
MP4s to be posted so I am not looking
at a dialogue box, inside an application,
inside a window, inside a browser?

 

It is understood now that it would have been better
to begin the Sketch at the origin center to
use circular symmetry as the basis for the
model design.

The six_point_star is renamed
seven_pont_star_trippy_241217 v1.f3d
and attached herewith.

This model is quite close to the design
vision. The only adjustment that is to be made
is to make the model deeper. That is,
the dimension between the star center point
and the bottom of the star tip, as shown
in this image
star_depth_dim_241217.jpg
is 8 mm.

In order to make room for PCB, battery,
and wiring the dimension between the
star center point and the star points
that would, if the star was place on a wall,
be bearing on the wall, would be increased.

To this end, at Modify > Parameters
the degrees Parameter was changed from
15 degrees to 45 degrees. This has the
desired effect of making the edges
of the star points more acute but
the undesired effect of reducing
the width of the points. And
the overall depth of the star
remain 8 mm.
Degrres_45_01.jpg

It is surmised that the reason why the star stems are thinner is because the
the radii coming from the center point are shorter.

 

Working on making these final changes.
Any ideas on an approach to making
the star deeper without reducing the
width of the points would be welcome.

Thanks.

Allen Pitts

Message 14 of 18
etfrench
in reply to: pittsallen

Slightly simpler method using two draft commands:

etfrench_0-1734466040890.png

 

ETFrench

EESignature

Message 15 of 18
laughingcreek
in reply to: pittsallen


@pittsallen wrote:......Would it be possible for the
MP4s to be posted so I am not looking
at a dialogue box, inside an application,
inside a window, inside a browser?...

Are you watching them in full screen mode by clicking in the lower right after you start the video?

laughingcreek_0-1734467669520.png

 

Message 16 of 18
pittsallen
in reply to: pittsallen

Hello @laughingcreek @TrippyLighting @etfrench, and the Fusion forum,

 

Appreciation shout out to etfrench for file 7Star.f3D.

 

The overall design concept is a hollow seven point star
with space inside to house a printed circuit board (PCB),
wiring and seven LEDs at the star points.

 

The following is not a step-by-step but somewhere
between an abstract description and a step-by-step
process to describe the
methods and commands used to get the final product,
7Star_241218_ETFrench_05.f3d, attached herewith.

 

The reason for this methods description is in the hope
that a similar description could be elicited on
how 7Star.f3D was created.


Methods Description

Mr. French's excellent model is solid so the first thing
done was to figure out a way to hollow out 7Star.f3D
Tried several methods to Extrude out the inside of
7Star that would create a plane parallel to and, say, 3 mm
inside the face of the star. No luck.

So, to hollow out 7Star three sketches were drawn and extruded

that created some space within the model.
7sTAR_HOLLOW_241218.jpg

To create the holders for the LEDs a Component called
LED Holder was begun, a Sketch called LED Holder
was drawn and Extruded as Body child to the LED Holder
Component.
LED_Holder.jpg

The seven tips of the star were then removed using
a sketch named ' Remove tips' and a Cut Extrusion
done to blunt the ends of the star points.
7Sstar_hollow_w blunt _ends_241218.jpg

The LED Holder Body was then attached to the blunt
end of the star point using the Modify > Align
command (JHackney provided a tip on this: After
the Align command is chosen, mouse over the face
to be aligned and hit the control button and
hold down the control button while choosing the
glyph of the plane required.)

 

The LED Holder Body was then copied and aligned
with the blunt end of the other six star stems.

 

Finally, a Sketch called 'Remove back for LEDs'
was drawn by projecting the Star body onto a
Sketch in the XY plane. A replica of a 5 mm
LED was created and fit into the LED
5_mm_LED_image_241220.jpg
Holder Component and based on measurements
the LED Holders and the adjacent Star stems
were extruded so the LEDs would fit up
LED_holder_241220.jpg
inside of the LED Holders and the LED
leads and wiring could pass into the
inside of the Star and to the PCB.

It is hoped that a description of how Mr. French's
7Star.f3d was created, similar to the description
provided herewith above may be elicited.
.

This is what has been garnered by studying
7Star.f3d.

First a Sketch of a triangle was drawn.

This is where it starts to get fuzzy.
The next command in the Timeline is
an Extrusion. But exactly what was Extruded
and how is not known.

The next two Timeline items are Draft1
and Draft2. Perhaps these Drafts are created
by saving the model, not sure.

The next timeline item is Mirror. It is
conjectured that the object that was
Extruded was half of a Star stem and
the other half of the Star stem was
created with the Mirror command.

The Circular Pattern command was then
invoked to create the remaining six star stems.
The Circular Pattern features was found
at Design > Solid > Create > Pattern > Circular Pattern.

 

Finally, the Modify > Combine command was
invoked to make the seven Star stems into
a single unit.

Is this a fairly accurate description of
the process employed to create 7Star.f3d?

What was the nature of the Extrusion done
after the Sketch and before the Mirror?

Thanks.

Allen Pitts

Message 17 of 18
pittsallen
in reply to: laughingcreek

Hello LaughingCreek,

I am hip to the full screen option.
This the result.Full_screen.jpg

 

Thanks.

Allen

Message 18 of 18
etfrench
in reply to: pittsallen

You're working way too hard.

  1. Start with Rule #1 and create a component for the main body.
  2. Joint the led to the holder.
  3. Combine the led holder to the first segment of the main body.
  4. Cut (keep tools) the led from the main body.
  5. Circular pattern the first segment.
  6. Combine them.
  7. Cut the pcb pocket.
  8. Cut the wire channel using a thin extrude.

Alternative to cutting the pcb pocket would be to shell the first segment before combining with the led holder:

etfrench_0-1734725182862.png

 

ETFrench

EESignature

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