Get negative/reverse part(s) from surface


I have troubles getting out the reverse (= negative or inverted) object fitted in a BoundingBox:

A … the surface model
B … BoundingBox around A

I want the BoundingBox to be splitted at least into two parts having the outer and inner contour on two remaining solid blocks.

What is the best way to do that if there are areas, where no clear separation is possible? Is it possible at all?


Hi Milling - the object has to extend through the box somehow, if I am reading your image correctly, you’ll need to add surfaces to all edges that do not penetrate the box. But, post your model, it will be easier to see what’s needed.


here comes the model.
NegativeSample.3dm (171.8 KB)
I already thought, that I must extend something/somewhere. But what best to do next? And would this work also with meshed objects?

Regards, Milling

Hi Milling - one thing that will make this difficult is that the surfaces do not actually meet where you’d think they might

I’d say you need to get the surfaces meeting cleanly, then make a bounding box (BoundingBox command.) Offset the BB a little (OffsetSrf) and then use Fin > Direction=Tangent to shoot some surfaces from all the ‘open’ edges out past the BB. Trim them with the BB and then to each other where they intersect. Then use all of these to split the box surfaces.


Hi MillingGuy

Here is my suggestion for your project (see work flow from below).


Step 1 - Your part needs a splitting line (parting line - P/L). The so called “negative” of this part will need to be split between a core and a cavity.

Step 2 - I did my P/L by using _Contour, then connecting the quadrants of the sections on the side (for the “wings”) and then split the part in cavity side (yellow) and core side (brown)

Step 3 - Used a combination of Ribbon, Sweep 2, Loft commands to build the cavity block. Notice that the part edges are a result of seal-off intersection of the cavity to the core plus a match between the core and cavity edges. I do not mean match as in Rhino command but rather a tool making match.

Step 4 - Showing the cavity formed part (yellow) in the cavity block

Step 5 - Showing the core (green) and lifters (blue). Lifters are needed to release the brown portion of your par from the core.

Step 6 - Showing the brown surface to be released by the lifters

Step 7 - Showing how the part is ejected by the lifters from the core

Step 8 - Showing a cross section illustrating the concept of the lifters at full stroke. That is when the part is fully released


That is an awesome illustration :slight_smile:

That would be an expensive tool. DFM should be a consideration, and there are many factors involved. It could be that a small change in the design produces a more cost effective part.

Probably some additional information is needed here before deciding on the type of tooling.

For example, if the requirement is for a 2 pc tool and the part must be completely solid and in 1 pc, it is unlikely this part could be made without changing the design.

1 Like

Hi Chris

Cool. Finally, something for me to talk about in an educated manner. I can never speak about Rhino issues with the same eloquence as my skills are miserable at best.

Here are a few assumptions and considerations.

  1. Part is molded and made of some plastic resin
  2. Yearly Volume: Under 50
    a. Make a silicon mold – only lasts between 30 and 100 shots, pending on complexity
    b. Choice of resin is limited to what can be liquefied and poured in the mold (gravity fed)
    c. Cycle time is in the hours: pour the liquid, wait to cure, eject the part, rework the part of imperfections
    d. Cost of mold: minimal (you could probably do it yourself at home)
    e. Rapid prototype shops could have this done for you at piece price deal, where you only pay for the part and not the mold
  3. Yearly volume: Under 1000
    a. Make an aluminum mold (visited with this shop molding aftermarket fascia’s and they claimed they could extract 50000 shots from that tool)
    b. The choice of plastic is now unlimited, but you now go into injection molding
    c. Pending on resin, you will need an injection machine of 3000T US (2700T Metric) – you do not find these everywhere
    d. Cycle time is now under a minute – compared with hours from above
    e. The mold will still be designed with bare minimum components, but will still cost over the $50,000
  4. Yearly volume: Under 10000
    a. Make a steel mold with minimum components (cheap is the word)
    b. All good things from the aluminum mold apply or are improved
    c. Cost is going up, but you now are almost a professional molder
    d. Best quality part
  5. One time off part
    a. Build a wooden core
    b. Buy a sheet of the required plastic and mold it over the wooden core with boiled water and hot air (what a mess)
    c. Worst quality part, good enough for a prototype


I think most people designing don’t want to be concerned with these things. Unfortunately, if ignored, manufacturing issues will surely present an unpleasant surprise.

I’m hoping that DFM is being taught in design schools, and even if one is not in an ID or Engineering program, I think it would benefit people who use 3D modeling for other purposes. My reason for this is I have seen on several occasions where there is some belief that any 3D model is somehow instantly manufacturable. I suspect this has to do with 3D printing.

1 Like

Hi Pascale,

I’d say you need to get the surfaces meeting cleanly

indeed… but it is just a sample I’ve done without any check. it should just illustrate an every days problem I have. and second, I still must also figure out, how to get surfaces from closed curves without loosing bounderies information. but that’s another problem.

Hi Costel,

Here is my suggestion for your project

uhh… thanks a lot for this work and demonstration. I’ve to walk through it and figure out, how you did this all. I’m not such close familiar with Rhino knowing each command and all its parameters
At all is demonstrates to me, that it isn’t just that easy :cry:

Much thanks, MG

1 Like