Kitchen design (assembly of same components with edit of their dimensions)

[Anonymous]

Hello everyone,

I am quite new on this software, I have done a lot of research but cannot find the trick... I would like to design parametric kitchens but I cannot find an efficient workflow.

I see a kitchen as an assembly of standard components like wooden boxes, drawers, doors, shelves, so I imagine :

1 - to design these components

2 - to draw a plan composed of simple squares

3 - to insert the components into the plan

4 - to break the links of these components and to adjust their dimensions according to the plan.

Does this make sense with Fusion 360?

My main issue is to define and insert the components in order they will fit to the updates of the plan.

I used to do it in Topsolid with boxes (the component is defined according to a box and the plan is composed by boxes). I understand Fusion 360 works with sketches, so I design each component according to a sketch, make it as a rigid group, insert it in the plan with a joint, break the link, and edit the sketch.

I am looking for the best way to catch the correct dimensions of the plan.
1 - If I define my components by dimensions, I will have issues to place and adjust components on squares which are not defined by dimensions (the "measure" tool do not updates when the plan is changed)
2 - If I define my components by parameters, I will have tons of parameters and will get lost.
3 - I chose to edit the component's sketches by making some lines colinear with the plan, it is a bit long but it seems to work. Do you agree?

I do not find a way to joint the components to the plan's sketch.
My joints do not follow the changes of the plans. Don't know what is wrong...

I have made a screencast to help you understanding.

Hope you can help.
Thanks a lot!

[Marco.Takx]

Hi @Anonymous,

I think for you it is interesting to install this add-in for Fusion 360

JoinerCAD 

If my post answers your question Please use Accept as Solution & Kudos This helps everyone find answers more quickly!

[davebYYPCU]

Sorry, reply is for @Anonymous ....

There was a lot in that video, that is hard to interpret, but Using your Example, I will call it a layout sketch, and (hollow box) component.

Make the layout sketch in the Root / top component. 

Import Component, 

joint component corner to sketch corner. (Joints need 2 Components)

Change component width parameter to equal the sketch parameter width, 

Change component height to sketch height.

Next component - repeat my steps 2 to 5 etc.

change layout sketch dimensions, to watch the magic.

Might help....

[Anonymous]

Thanks @Marco.Takx, I already use Joinercad which seems to be really efficient to get BOM but does not help in designing. Its software developer made an add-in called Woodwork for Inventor which seems to be perfect for designing kitchens, but it is way too expensive and works only on Inventor...

Thanks @davebYYPCU, I think I already do what you are suggesting... I might do something wrong when I use the joint tool...

[davebYYPCU]

Not sure why yours does not work, I can do as I said.

Change the values of any of the first 6 parameters. Values must be greater than 10mm

Might help.....

[Anonymous]

Hey @davebYYPCU , thanks for your quick answer! I wanted to make many tests before answering you and it took some time...

You model helped me a lot to understand what is wrong with mines. I still have an issue with the way I make joints.

I have tried to redo the joints on your model on the 2nd and 3rd boxes.

- 3rd box : the joint is on the left down corner of the box and of the main sketch, and have a problem when I change the dimensions.

- 2nd box : the joint is on the center of box' sketch and of the main sketch, and I don't have any problem!

When I check the 1st box, I see a joint on the left down corner... How have you done it?

Thanks a lot

[davebYYPCU]

What I did,  - very simple.

Layout sketch, with dimensions - when making dimension 1, type in "H1", for the value, sketch will say FX:80.00

and Dimension 2 type in "L1" for the value, sketch will say FX: 111.00

repeat for other 4 dimensions, parameter name for value. (L2 H2 H3 L3)

For component 2, first box, sketch centre rectangle, and

dimension, type in H1, for the value and type in "L1" for the value,

make 4 box sides, use Thickness parameter (I used Shell command.)

repeat for 2 more boxes.

Layout sketch is component 1, fixed to origin, and can't move.

Joint Component 2, rigid, and left lower corner of box front goes on lower left corner of layout sketch.

Joint Component 3, rigid, and left lower corner of box front goes on middle lower left corner of layout sketch.

Joint Component 4, rigid, and left lower corner of box front goes on right lower left corner of layout sketch.

Open Parameter window, and change any value in top 6 user parameters.

Model will behave as expected.

Might help....

[TrippyLighting]

@Anonymous The "feature" you are looking for is called "Configurations" in other CAD systems (Solid Works, Alibre Design, ZW3D). Autodesk Inventor I believe uses a different name for this but it functions the same.

Unfortunately, Fusion 360 still does have that feature!

In a nutshell, it allows you to assign a set of parameters e.g. a set of dimensions to a single ID, the Configuration.

When you change between configurations, it updated the values of all the parameters assigned to that configuration.

The plugin Sheeter might help some with this.

[Anonymous]

@TrippyLighting Thanks, I will take a look at it!

@davebYYPCUThanks for your explanation, I tried to follow your steps and still don't get it...
I've made a screencast to show you what I do. I might click wrong somewhere...

I've uploaded the file to let you check (1st box works, 2nd doesn't if you change the parameters).

Thanks a lot!!!

 

[davebYYPCU]

I checked your file, as you say box 1 is behaving, but because both of the sketches are used for the Joint, the front of box is not aligned to master sketch, it is both sketches that are aligned.

Box 2 joint, I can not find what you selected for the joint, in the layout sketch, but if you edit that joint, you can reselect the front middle sketch point, making sure the joint disc, is flush with the sketch.

Might help....