Shelling issue...

Rank: 1

Eli

Newbie

posts: 0

Registered: 2004-10-28

Message 1 of 12

 Shelling issue...
05-11-2004 01:37 . pm | View his/her posts only
I am having a strange issue with the shell operation. For a good while, when I shelled something, I could make a surface turn into a solid of certian thickness. This is good. Now, it seems that I can only shell into what appears an offset surface. This is not what I want...but I can't seem to get back to simply thickening something. I can add side faces, which makes it appear like a solid, but as soon as I trim the shape with something else, it becomes clear that there is nothing inside between the two faces. What is going on here?

Rank: 1

Eli

Newbie

posts: 0

Registered: 2004-10-28

Message 2 of 12

05-11-2004 01:42 . pm | View his/her posts only
Ok....it looks like that if I use a combine shapes trim vs a trim to faces trim I get a solid versus to faces. Still seems a bit odd to me though if the purpose of shelling in the first place was to create a solid....why would a trimming operation negate that?

Rank: 1

ChrisWard2k2

Newbie

posts: 2

Registered: 2011-11-22

Message 3 of 12

05-11-2004 02:04 . pm | View his/her posts only
Hi Eli

During the trim op, VX has been unable to build a new side face. If you are working on a large-scale part, then this is likely to be related to computational tolerance. The default tolerance in VX is 0.01mm. Go to Edit Preferences and change the tol to 0.1mm - see if that makes a difference. Note, a computational tolerance is used by the system to determine the definition of the shapes - i.e. whether a computed edge gap should be displayed as a gap. It is not an engineering tolerance.

Rank: 1

Kevin

Newbie

posts: 0

Registered: 2004-4-26

Message 4 of 12

08-11-2004 04:31 . am | View his/her posts only
Chris,

You say that the tolerance within VX is defaulted to 0.01mm but it is not an engineering tolerance but a computational tolerance to determine if the system can define the shape or not. Is this not the same thing?? If it is a display tolerance then surely this would not affect the shelling (or indeed any other) operations?

How does this affect modelling reliability for exporting the VX data to other systems. My experience of other systems is that reducing the modelling tolerance reduces the accuracy of the shapes and leads to gaps when importing into CAM systems. Certainly in Parasolid and ACIS based systems you can reduce the tolerance for modelling to "force" an operation (tends to be called tolerant edges in ACIS for example), but in ACIS the general modelling tolerance is something like 0.000001 modelling units. In a previous life using Think Design tolerance switching was a frequent requirement to make shelling and filleting work BTW!

Perhaps you could explain to us switchers how VX handles this and what we need to watch out for?

Thanks

Rank: 1

Kevin

Newbie

posts: 0

Registered: 2004-4-26

Message 5 of 12

08-11-2004 04:34 . am | View his/her posts only
Sorry I just read your post again (its Monday morning and the coffee hasn'r kicked in yet!) and I think you are talking about the scale of the part relative to the default modelling tolerance?? ie. a big boat needs a bigger base unit to work whilst a bottle closure (like I'm working on now) is much smaller? Is this correct?

Rank: 1

ChrisWard2k2

Newbie

posts: 2

Registered: 2011-11-22

Message 6 of 12

08-11-2004 07:55 . am | View his/her posts only
<DIV>Hi Kevin

Well, broadly speaking, yes. You can use your engineering tolerances to judge your choice of computational tolerance. That is where the relation ends. The computational tolerance is concerned with shape status. For example, If you have got a "gap" that is intentionally 0.01mm wide, it is right on the default tolerance value -so, the system may struggle with this. i.e., should the system consider the gap to be intentional and therefore show a gap, or should the system regard it as uninteniontial and show the gap closed (and therefore allow the shape to be regarded as a closed volume or Solid)?</DIV>
<DIV>
Now of course, the size of the object being modeled has a distinct effect on the choice of computational tolerance. For most other CAD programs, it is a critical subject because you can only apply one computational tolerance for the entire model. VX is different, since you can apply a tolerance that is appropriate to a feature of the model. The aircraft industry for example manufactures some very large scale machined parts, yet those parts also include tiny details. VX allows you to set a small tolerance for small features on large parts - we call this proximity tolerancing. Export files from such VX models might make receiving CAD systems uncomfortable - in a similar way, not all CAD systems can cope with the sophisticated surface shapes that VX can define. What can I say? The companies that require such data need to invest in a system that can really handle it - I suggest that they buy VX!




</DIV>

Rank: 1

Kevin

Newbie

posts: 0

Registered: 2004-4-26

Message 7 of 12

08-11-2004 09:11 . am | View his/her posts only
Very interesting Chris,

One thing I'm still a little unclear on though is the 0.01mm "limit". Are you saying here, that VX is not optimised for defining shapes where the part tolerance (eg for snaps or mating features) requires accuracies better than 0.01mm? I accept that for most applications this is acceptable but for tiny high precision mould features this becomes important. If this is the case can the tolerance be increased to 0.001 say?

Rank: 1

Eli

Newbie

posts: 0

Registered: 2004-10-28

Message 8 of 12

08-11-2004 10:24 . am | View his/her posts only
This is interesting. When I export files from Multisurf, the program that I use for developing hull shapes, the default tolerance there is .00019 or something. Kevin is right in that that seems to be a bit overkill for my purposes. The reality of the boatbuilding industry, even those that are working from CNC machined tooling, is that kind of tolerance is not really achievable, nor is it desireable in almost all cases. Now, when I export, I am exporting a file that I drew up in imperial units. Maybe I'm wrong about this, but whenever I'm in VX, the setting of .01 seems to be the default tolerance for inches as well as mm.

Rank: 1

ChrisWard2k2

Newbie

posts: 2

Registered: 2011-11-22

Message 9 of 12

08-11-2004 12:37 . pm | View his/her posts only
Hi Chaps

I did not say 0.01mm is a limit, but that it is the default. You can change the default via Utilities/Configuration/General. The minimum value is 0.001mm.

Also, before exporting, it is possible to change the computational tolerance (for the export), by temporarily changing the value in Edit/Preferences.

For the curious, I attach a model of a 50x50x50mm "cube". Now, the model has a deliberate 0.05mm gap on one face (green face). The geometry was created at tolerance of 0.001mm. Step through the history, and select the Surface feature for edit. Go to Edit/Preferences and change the tolerance to 0.1mm, then <OK> the feature. The last two history steps erase the line used to define the 0.05mm gap, and change the face colour. With the history complete, you can observe that the system now regards the geom as a Solid. If you step through the history again, and change the tolerance back again, you will have an open faceset again.

Rank: 1

Kevin

Newbie

posts: 0

Registered: 2004-4-26

Message 10 of 12

08-11-2004 01:03 . pm | View his/her posts only
Thanks Chris,

That explains things better. I was a bit concerned about the 0.01mm value as this seems a bit high for some work - not so much the everyday stuff but for highly detailed items and those requiring manual data entry onto wire profilers (yes there are many who prefer to do this - they do the job fantastically well and I respect them for it!) where you have perhaps a complex profile made from arcs - the arc centres often need to be positioned to three decimal places or they don't tie up properly.

So, without being pedantic though,what is the geometrical limit that VX can work to accurately?

Thanks for your valued input here!

Rank: 1

ChrisWard2k2

Newbie

posts: 2

Registered: 2011-11-22

Message 11 of 12

08-11-2004 09:46 . pm | View his/her posts only
Hi Kevin

I assume you mean the smallest entity that can be reliably defined. Well, I don't have a black and white answer for that, but VX can get close to it's tolerance so you are looking at entities that are "not much bigger" than 0.001mm (For example, I just modelled a 1mm x1mm x 0.0011mm wafer). UK VX customer, Amchem, produces tiny holes (measured in thous and not cylinderical!) in aircraft engine turbine blades. Their customers include Rolls Royce and Pratt and Whitney. The holes are produced using purpose-built EDM machines built by Amchem, the task is that special. It is a very serious business - if a turbine blade were to fail.......So, Amchem's only criteria when purchasing CAD/CAM was "can it do it?". VX was the only one they found that could.

How do you output the data for manual input on the wire profilers?



Rank: 1

Kevin

Newbie

posts: 0

Registered: 2004-4-26

Message 12 of 12

09-11-2004 05:21 . am | View his/her posts only
Thanks Chris,

That answers my questions completely. If VX can handle that level of accuracy then I see no problems with anything we do. As for the wire issue this came up first when working with a new supplier a few years back (when we were doing work for a customer and needed to use SolidWorks - their request). The actual components were machined stainless parts for a "life critical" application (can't say what). We gave them data from SW at first as profiles for wiring (as SW drawing files) but they had issues programming the CAM (they had just purchased a SW based CAM system) from these so we ended up supplying dimensioned drawings from their requested datum start holes. I mistakenly supplied the dimensions to 2 decimal places, but this wasn't accurate enough for some of the profiles with LOTS of tangent arcs. The most detailed was a 4 decimal place drawing which worked OK. Maybe the supplier was being a bit pedantic but the job was an expensive one and the timescale was very tight - no margin for mistakes.
See also