Hi
I work in field of furniture.
Currently, I start with Part (ipt) then Make Component. they will create new Assembly (IAM). What if I change design, add new solid. I think about 2 way:
1st way, I will create new Part in Assembly file, but I will not able to substract with other object.
2nd way, I come back to first Part file and draw new solid. then I can substract with others (I want to keep solid after substract)
Need advice to good practice workflow in field of furniture.
Thank
Travis
I am not sure if I follow this correctly but as JDMather mentions you can use multi solid body part modelling and you can combine and then select to "Keep Toolbodies" and if you use make components on a multi solid which has already been created just make sure to save over the existing Assembly and Inventor will only create and add the solids which don't exist in the old assembly.
If you select solid bodies which have already been created Inventor will show them as blue line items as they will essentially be skipped. below is what it will do.
Hi Travis,
Inventor is a distributed design CAD tool. Each ipt file contains the geometry and the iam file aggregates the ipts to create the assembly. Any cross-part/cross-component workflow can be less straight forward.
In your case, I suspect you may leverage Copy Object workflow. Edit the target part in place -> Modify section -> expand it -> Copy Object -> select the tool part; set output as Surface -> check "Associative." Now, you can use this adaptive body to cut the target part.
Many thanks!
Hi Travis,
There are quite a few videos showing the workflow. Here is one.
https://www.youtube.com/watch?v=5smTHeCIbSQ
The process is very straight forward. It is literally the way I described it. If you got stuck, please feel free to share an example here. Forum experts can help take a look and propose a better solution.
Many thanks!
Thank @johnsonshiue
It worked well.
By the way, what different between these setting?
If I select setting Surface or Composite they will have Associative, they will update if I change sketch.
If I select Solid they will not have Associative and they will not update if I change sketch.
Follow this method, I think about workflow:
1/ Start with Assembly
2/ Create/ new Part
3/ Sketch and make model in this Part.
4/ If need to Substract object, Copy object as Composite with Associative.
5/ Use Sculpt feature to Substract object.
Is it good practice?
Thank
Travis
Hi Travis,
Copy Object is like a combo command. It offers quite a few workflows. When the output is set to the Surface or the Composite (option 1 and 2), the Associative checkbox is enabled. This is the "Adaptive" body workflow. Essentially, the body geometry from the source part can drive shape change in the target part within this particular assembly.
I personally prefer Surface output since it is more versatile in terms of modeling operations. Composite is a group of mixed bodies (surfaces and solids). It is more for representing the source part, not for modeling operation purpose.
The option 3 and 4 are both non-associative solid outputs. The difference is that #3 just copies the solid body from its position in the assembly to the target part. There is no link established between the target part and the source part. The #4 option does the same but places the copied body to Repair Environment (a persistent, non-feature-based, and non-parametric environment to fix imported body geometry), since Copy Object command can also copy solid bodies within the target part itself, not just across the part.
I notice you have quite extensive Fusion experience. The major difference between Fusion and Inventor is that Fusion tends to manage all component definitions within one design, while Inventor manages individual parts and assemblies as files. Each component can stand on its own or be referenced in another component. There is distinct boundary between two components (two files).
Many thanks!
