Creo 2 Parametric Syscol.scl file options

[bpenza]

Does anyone have a listing of options that can be put in the syscol.scl color file? we are moving from WF4 to Creo 2.

One of the technicians at PTC stated that their isn't any documentation.

Thanks in advance,

Lance Lie

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[TomD.inPDX]

You are working with a very small bolt. It could be in the accuracy settings. Try changing the pitch to a larger value and see if that lets it work.

In general, these work as expected but sometimes it gets lost. Is the value of L1 the same as the pitch? This can cause issues and can be resolved by stepping the triangle outside the bolt face and increasing L1 but manage the ID of the cut. This will create an overlap in the spiral but will eliminate the tangency issues.

The trajectory is simply a guide. The axis is a key element. Just know how your sketch will interact with the trajectory.

When I define a bolt like this, I try to leave the appropriate flats. Making the widths of the flat the same inside and outside is the challenge. The theoretical sharp of the thread is always slightly larger than the specified screw size. Below, the pitch is also .8:

[dschenken]

Where's the challenge?

Sketch a construction line that is at the top crest and bottom crest location and another that is just below (oriented per your diagram) the bottom crest location. These construction lines will be constrained to points on the OD so that the geometry lines can extend beyond the body of the screw.

The distance from the last construction line and the upper one is the pitch. Set the distance between the last construction line and the bottom crest location to be the same as the minor diameter flat and they are automatically equal. This will replace the 0.8 dimension.

Cutting screw threads in models is an interesting exercise, but they are computationally expensive and provide little feedback for design purposes. For example, they don't well record the minimum and maximum threaded lengths, which a pair of datum curve circles can do. Threaded length range is useful to display that there is enough thread engagement.

I really wish PTC would make use of solid surface characteristics, such that one could apply a thread pitch and minor diameter and, when assembling, one could get feedback that the mating surface matched, and ignore interference between the major diameter solid surface of a screw and the minor diameter solid surface of the mating nut while not ignoring clearance problems with non-threaded surfaces. We're only 13.9% into the 21st Century and meaningful checks that don't produce a bazillion false positives are a lot to ask for. Yes, I know about cosmetic threads, and they don't offer this ability, and aren't particularly cosmetic, tending to show through solid features needlessly.

[TomD.inPDX]

(the sketch already constrains equal flat areas with the two equal diameter reference circles. I use the ID from the provided cosmetic thread to determine the offset)

Although it has always been PTC's stance that threads need not be modeled, they work really nice when grown using a quality 3D prototyping system when you don't have the particular tap on hand. They also help in some instances where you want realistic images or diagrams where you want to distinguish between threaded holes and through holes.

A great improvement to the software would be to allow toggling between cosmetic and actual threads. You can add to the votes if you can access Ideas here: Thread ideas: modeling and drawings

[dschenken]

=Clever, but not obvious control.

The construction line method directly controls the crest and root flat widths.

The threaded holes have lead-in chamfers, so that's easy enough.

As I said, its an interesting diversion, but not of much use in design by which I mean engineering design, not product illustration images. If it is to look good, a helical spiral datum curve is faster to create and won't fail to regenerate. Maybe use a decal texture?

If it directly drives a manufacturing process, there's not much else to do, but the vast majority of helical threads are manufactured either by dedicated tooling such as taps and dies or roll-forming, or by canned manufacturing cycles that do not depend on a surface model. Solid modeled threads are costly to open, copy, regen, and display. Maybe it's not so noticeable for little assemblies, but build an assembly of a few hundred .5 inch .190-32 screws and see if there isn't a bit of a hit on performance.

Same goes for solid modeling of pierced and expanded metal, grating, woven wire screens, knurling, honeycomb, and other items or features that are not fabricated in detail based on the model. It's easy to add 1% or more to the CAD cost of a project for something that adds no value to the execution of the project.

Again - 13.9% into the 21st century and PTC still doesn't supply tools to determine the detailed performance affects of various modeling techniques in terms of CPU cycles spent, memory allocated, and triangle generation/memory for graphics display.

[ReinhardN]

Hello Brett

#4: If your sweep cut intersects itself the feature will fail. You can check it by switching your feature to surface.

Reinhard

[TomD.inPDX · Accepted solution]

There is a caveat to that, Reinhard. If this occurs on the surface of the part being cut, yes it will fail, but if it is beyond the surface it works. So yes, it can intersect itself except under certain circumstances. I know there is a lot more to it than I can explain, but for the most part, the failure is tangency and accuracy rather than a simple rule.

When the edges are very close to tangent, you will fail on accuracy; when the sweep tries to share the centerline, it will likely fail; there is a difference between Section orientation - Through axis of revolution|Normal to trajectory as well. <<== this one gets many people when defining a Helical Sweeps... In springs, for instance, the wire needs to remain round and the orientation should be set to Normal to Trajectory.

In general, it is a bit of extra work to get a successful helical sweep if you want a textbook theoretical thread. Once we get around this, they seem to rarely fail; or at least, we know what to do about it in short order. But one thing I won't except is to have the software tell me what I can't do. One way or the other, I do get exactly what I want.

This will work for the original question where the sweep sketch is on the edge of the cylinder, and the equilateral triangle is normal to the revolve axis... It also controls the thread width the same as the pitch.

[dschenken]

Feature creation wise, features aren't actually self intersecting, i.e. a feature can't cut itself.

The most difficult part for feature creation is dealing with coincident surfaces, particularly for material removal. A tiny numerical difference separates removal of a surface and generation of a thin sliver of material. That's why it is more reliable to extend feature geometry because it avoids coincident surface evaluation.

This doesn't usually affect nominally flat geometry**, but curved surfaces are internally represented by a large number of small triangles. It is more likely that the new feature triangles will not exactly match those of the existing feature surface triangles, leading to difficulties in comparing them and leading to regeneration failure. Changing accuracy can sometime change the situation - it causes the creation of a new set of surface triangles that conform better or worse to the ideal surface. Failing features may work and features that did work may fail when accuracy is changed.

The reason that creating surface geometry instead of solid geometry always works is that no comparisions are done.

As Antonious shows, if the solid feature doesn't intersect the existing solid surface geometry there is also no way for the coincidence comparison to fail. It will result in oddities, like the volume of the part can be smaller than the volume of its features.

** I've had occasion to try to remove a .005 depth patch from a large casting and it failed, but using the same sketch on an plane offset by an inch to a depth of 1.005 inches allowed it to work just fine.