How to "stick" two different bodies together?

[Anonymous]

Hi there,

I am relatively new to Fusion 360 and attached is the model I am working on.

The model unit should look like 7 interconnected balls "sticking" together. Therefore, my question is: How to move the spheres so that they all stick to the center sphere? Meaning, there should be no gaps between the spheres.

I also wish to parametrize all the holes (12 on each sphere with the same diameters) based on the diameter of the sphere, so that the hole is always 1/3 of the diameter of the sphere and the hole should change accordingly when I change the diameter of the sphere. However, I do not know how to parameterize the diameter of the sphere. I tried "compute all" and there is no diameter of sphere in it, nor the diameter of the holes.

The final step of the modeling, I think, is to use the pattern function to create a rectangular slab, with all the spheres "sticking" and interconnected with each other. I suppose that is entirely possible?

I truly appreciate your help!!

Jason

[Anonymous]

sorry, attached should be the files I want to show you guys!

[Pavel_Holecek]

Hello,

There is possible to use Circular Pattern on components and parametrize a sphere diameter and distance spheres. I attached an image where is possible to see how to show Parameters.

Regards

Pavel

[Pavel_Holecek]

Hi,

I forgot to mention that I use Assemble Joint to fix two sphares for particular distance. You can Find it in Toolbar->Assemble->Joint .

Regards

Pavel

[San_Escobar]

Hey jasonchenscie

I have put together a simple screencast aswell, to give you another idea how to go about to achieve such features in different way from t_holep

Somehow it didn't included the audio commentary. Sorry!

HTH, enjoy.

[Anonymous]

Hey there! thank you so much for your video! I have another problem - do you know how to create the hole on the contact points of the sphere? As you might be able to see in my attached png above, the spheres are interconnected with holes. What I did was drawing a circle (to be extruded as a hole) at the center of the big circle (sphere) and align it so that the line I draw goes through the center of the circle (to be extruded as a hole). However, when I tried to redo this modeling by following your workflow, I can't seem to be able to align the circle (hole) so that the green axis/line goes through the center of the circle (to be extruded as a hole). Attached is the new screencast describing the problem. Thank you so much!

Jason

[Anonymous]

I used my old model and the pattern function to let the spheres "stick" together... however, when I tried to combine the center sphere to the C-Pattern 1 Group, it shows this error shown in the attached 3.png. Do you know why and how to solve this? Thanks so much!

And also... an easier way to create holes at the contact points would be very helpful too!

Jason

[Pavel_Holecek]

 Hi Jason,

Sorry for this problem, I tried it with similar model like you have and I am able to reproduce it - therefore I logged new issue to our tracking system (FUS-18022).

Pavel

[LMD001]

Hello Jason,

Had a go at the spheres, not sure if this is what you want as result.

I had to do some Moves at the end to align the holes, I missed that you wanted them aligned.

Feel free to use the file.

Best regards,

Ludo

[Anonymous]

Thank you so much for your reply! It somehow says "opening of local files is not supported".

I actually figured the Move out earlier, the only problem left right now for me is the dimensioning of the circle after I move them. Somehow I cannot sketch dimension on the circle (hole) at the contact point....I need to dimension the all the holes because I want them to change accordingly with the diameter of the sphere 🙂 

The cloud service is down for maintenance right now, so I couldn't do a screencast.

Again, thank you all for your help!

[Anonymous]

Hi Pavel,

I wonder if you have any insights about sketching dimension on objects that are not on the x plane?  Somehow the "sketch dimension" function does not allow me to select the circle I highlight in the attached file. I even tried drawing a line tangent to the center circle, dimension it, and draw the circle by using the two points of the line. However, after I moved the circle (so that it is tangent to the center circle), the dimension of the line disappear. I wonder if I have done anything wrong?

I truly appreciate your help!!

Jason

[LMD001]

Hello Jason,

Took another approach to the spheres, this time with components and rigid joints.

The sphere diameter drives the hole diameter and the sphere wall thickness, you can change this in the Parameter window "User Parameters".

Here is a screencast: http://autode.sk/1AEE57m

Again feel free to use and modify the file.

Hope is of any help.

Edit: to use this file you have to download it first and then upload it to your account, it is how Fusion 360 works.

Best regards,

Ludo

[Pavel_Holecek]

Hi Jason,

I am not sure if I really understand your problem.

According to your screen capture you have two sketches – one sketch is in XY plane and second sketch is in XZ plane. And you want to use dimensions between these two sketches, right?

If you have an active a sketch (sketch is a plane – XY, YZ, with an angle, …)  then you can use dimension in this sketch only. Other geometry is possible to use for dimensioning in orthogonal projection. In this case I can recommend you to use ‘Project’ command. When you are sketching you can use this command (this command is possible to find in Toolbar -> SKETCH -> Project/Include->Project ) to project an existing geometry (body, construction , other sketches) to your active sketch. Projected geometry is possible to use for dimensioning and this geometry is associative with parent source.

Let me know if this is not answer for your question. If not, could you share a video with the problem?

Thank you a lot

Regards

Pavel

[Anonymous]

Hi Pavel, 

Thank you sooo much for your reply!

Let's refer the small circle that is "tangent" to the center circle as "side circle"

this is the video https://screencast.autodesk.com/main/details/f1956dc0-f30f-48ec-a9d9-021725ae1c17

I have next to no idea why there is a sketch 5, because as you can see in the video, when I selected sketch 5, nothing seemed to be selected. And when I selected sketch 1, everything including the side circle was selected, and when I tried to edit the sketch of the side circle, I could not select it by using the "sketch dimension" command. I also am not sure how to use the "Project" command to solve this problem..

Thanks,

Jason

[Anonymous]

Hi Ludo,

Thank you so much for your help and I truly truly appreciate it!!!! It would also be very nice of you if you could share how to generate this model. 🙂

Thanks,

Jason

[Pavel_Holecek]

Hi Jason,

this is really interesting. Do you have steps how to create such a sketch? And could you share your design ?

thank you a lot

Pavel

[Anonymous]

Hi Pavel,

this is the link to my sketches: https://myhub.autodesk360.com/ue29a8ac6/shares/public/SH7f1edQT22b515c761eeff0071b33b5bdc8

Let me see if I could duplicate this error by redoing everything...in the mean time you could try to play around with my file above.

Thanks,

Jason

[Anonymous]

Hi Pavel,

This is the video of how I created my sketch: https://screencast.autodesk.com/main/details/9679a69e-73ca-41b1-90b9-8596f5c1afd6

I also attached a screenshot of this design.

Thank you so much for your help,

Jason

[LMD001 · Accepted solution]

Hello Jason,

OK I'll have a go at a step by step.

Mind you this is the way I did this, in modelling, many roads lead to the same result, so my way is not necessarily the "best" way.

Here we go;

Start a New Design.

Step 1) Make a New Component,

Step 2) Activate this component,

Step 3) Save document.

Step 4) Create Sphere at Origin Point,



Notice d1 is the Diameter of the Sphere in the Parameter Table.

Step 5) Shell the Sphere with a wall thickness of d1/20 you can change this to suit your design,

Step 6) Create Sketch on the red/green axis plane,

Step 7) Circle on the Origin Point Diameter d1/3, then stop sketch.

Step 8) Extrude Cut the Sphere with the circle, use the settings as shown,

Step 9) Circular Pattern this extruded feature,

Choose the Timeline feature (extrude cut) as Object, the green axis, the features icon as Pattern Type, 3 occurrences.

Step 10) Plane at Angle,

Choose an angle that suits your design,

Step 11) Create a Sketch and a Circle (d1/3) at the Origin Point, stop Sketch.

Step 12) Extrude Cut this circle with the same settings as step 8, Circular Pattern this feature with the same settings as step 9.

You should end with a component like this,

This component has 12 holes 1/3 of the sphere's diameter.

When you change the diameter of the sphere in the Parameter Table, the holes will reflect this change (d1/3).

Will make part 2 (inserting components and user parameters) later today.

Hope it is of any help.

Best regards,

Ludo

[LMD001]

Hello again Jason,

Part 2;

Start New Design.

Step 1) Insert (right click on the saved component in the Data panel) the sphere you created earlier.

The Component will insert at the Origin Point.

Step 2) Rigid Joint on Sphere an Origin Point. This step is needed to "lock" the sphere in place.

Grounding the component seems to work initially but when you insert a second component the ground is lost. Not sure why.

Step 3) Insert another Sphere like in step 1. Move the second Sphere along the blue axis.

Step 4) Rigid Joint between the connecting holes, the first object selected will move.

Step 5) Circular Pattern the second Sphere around the green axis, 6 occurrences.

Step 6) Rigid Joint the remaining connected holes.

Step 7) Create User Parameter for the Sphere's diameter (d1 and d1_1).

Step 8) Change User Parameter Dia_Sph (you can use any other name), and see how the model reflects these changes.

This concludes part 2 of 2.

Again feel free to use and modify the attached files (download to your local drive and upload to your Fusion 630 account).

Hope this is of any help.

Best regards,

Ludo