Heal Geometry on Unparameterised Bodies / Sheets

[doncasters]

Good morning,

I am using NX8 currently and most of the work we do with it involves bastardising unparameterised bodies (from .igs and .stp files supplied by customers).
More often than not the first thing we have to do is a sew operation to create a solid. Sometimes straight forward, but sometimes an HUGE amount of work is involved in rebuilding to resolve disjointed edges, missing surfaces etc.
Analysis > Examine Edges works well to highlight problem areas. But obviously contains no remedy.
File > Export > Heal Geometry has so far always proved unsuccessful. Possibly because these files always stat unparameterised?

Does anyone have any other suggestions?

Many thanks.

 

[JohnRBaker]

Whether a model is paramaterised or not will have no effect whatsoever on whether 'Heal Geometry' works or not. You may need to play with the part file's modeling tolerance and the 'Tiny Tolerance' to get any results.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[doncasters]

I don't understand the relationship between these tolerances...

I have 2 sheets which overlap by 0.0027. I have used the default sew tolerance of 0.001 and adjusted the Heal Geometry tolerance both higher and lower than than the mismatch - 0.003 & 0.001.
Neither has made any discernable difference to the resulting part.

What should I expect to see from a successful heal geometry? I start with a sheet body that is comprised of multiple sheets sewn together, but some mismatch prevents it from being a solid.
> Heal Geometry.
Upon opening the _hg file should I expect to find a solid body? That is what I am hoping for, but maybe I am misunderstanding this function?

Thanks.

 

[jerry1423]

Cal you show a pic of the overlapping edge?

 

[JohnRBaker]

No, 'Heal Geometry' does NOT convert sheet models into solids even if that might be topologically possible. What 'Heal Geometry' does is attempt to REPAIR individual bodies whether they are sheet OR solid bodies. The idea it to first remove faces which are very small, often smaller than what the modeling tolerance is set to as these small faces can interfere with blending operations and other operations which depend on clean and unambiguous face edges. Also, these very small faces can interfere with faceting tasks including rendering or when generating Finite Element meshes. They can also disrupt the creation of toolpaths and such.

Another thing that 'Heal Geometry' attempts to do is replace complex faces, usually NURB's, with simpler geometry if possible. For example if a face is actually planar but is represented as a NURB these faces can be replaced with a planar patch. The same is true for faces which are, for all intents and purposes, cylindrical, conical or spherical. The idea is to get both 'cleanest', as in no tiny faces or ambiguous network of edges, as well as the 'simplest' possible model, in that if a face can be represented as a canonical form rather than a NURB or B-face then it's replaced with the appropriate simpler geometry. Often these operations are performed BEFORE a final sew operation is attempted in the case of a part file consisting of several multi-faced sheet bodies that need to be converted into a single solid body. Or when you already have a solid body, but for whatever reason, is of poor quality.

But like anything, truly bad models are often beyond repair or saving and while this tools can be quite effective, it can't produce miracles. Sometimes it's not possible to "turn a sow's ear into a silk purse".

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[jerry1423]

Maybe I can give a tip here to fix that edge.

Try to create a face blend (You can make it small or any size you want because size doesn't matter much here) between the two surfaces and make sure everything sews together.

Then delete the face of the face blend using syncronous modeling->delete face

NX will then trim the edge of the touching surfaces to its tight tolerance, not the looser tolerance that was used when they were created.

Then remove the parameters from those sheet bodies if you need to.

 

[loki3000]

hey john
in another thread i've read about nx's automatic surface capabilities (from scanned data). how would one go about creating an editable parametric model from that?

 

[JohnRBaker]

Well there are several different tools to help reverse engineer objects such as creating sheet bodies from point clouds or faceted models. Also there are tools that will try to automatically convert a series of sheet bodies into a solid body, but in ALL of these cases what you'll end up with a solid/sheet 'feature' but there isn't anything that you could consider as being 'parametric' about it. Now you could edit the resulting body, often as if it were a 'parametric' model, by using Synchronous Modeling techniques.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[doncasters]

Now I have a clearer understanding of the heal geometry function I think it is time to admit defeat - it seems I have been supplied a sows ear, and was expecting too much from heal geometry. We manufacture some complex castings and resolving all these issues in order to interrogate the mass can sometimes take days. We use the synchronous workaround mentioned above. Just for the sake of getting a solid sometimes just throwing an N sided surface into a gap can help too - but it never 'feels right'.
I guess we just carry on doing what we are doing, and asking for parasolids instead of IGS files where possible.
Thanks for the education !

 

[MikeHyde]

If you have a lot of data, you might find CADdoctor from Elysium useful for cleaning it up. I have used it to repair large panels created in a French CAD system. The parts took a few hours to fix and there are plugins to easily import the repaired solid into NX.

Mike Hyde

http://www.astonmartin.com

NX8.5 with TC9.1

 

[Toost]

I have looked ( Not bought yet, no experience of my own so far) at CADFIX from

http://www.transcendata.com/

due to issues with DWG 3D data. ( Crap data ...) Looks promising.

Regards,
Tomas