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Cosmetic feature in start part

GrahameWard
4-Participant

Cosmetic feature in start part

In my old position we used a start part for all our new ProE parts. It had default datums planes etc., but we also had a cosmetic feature, a sketch of a circle about an inch in diameter. It was never used for anything, and at first I used to just delete it from my parts, and everyone else would jump on me and tell me to leave it in. Their explanation was that it affects the software's perception of the scale of the model or something. The idea is that even if the model becomes larger than the cosmetic feature, with the addition of later features, it somehow is pinned to a particular "regeneratability" because it started out as a particular size. (I never knew files had memory.) I should add our parts were mostly around hand-sized, so the cosmetic circle, while usually smaller than the final part, was never an order of magnitude smaller.

This always sounded like a load of dingo's kidneys to me, but after that discussion I would leave it in like a good boy, because it's not about me, is it?

Has anyone else heard of such a thing? Do you do something similar in your start part? I ask because I am making some templates for my current job and wonder if I should put this feature in it. Creo/Elements 5.0.


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20 REPLIES 20
Inoram
12-Amethyst
(To:GrahameWard)

I thought some people do that just because when they start sketching they want the sketch area to be closer to the size parts they are drawing.

I would think other then that, a better idea would be to turn and set absolute accuracy instead of relative.

GrahameWard
4-Participant
(To:Inoram)

Matt Griswold wrote:

I thought some people do that just because when they start sketching they want the sketch area to be closer to the size parts they are drawing.

That makes sense. No reason not to delete it again afterwards, though.

I would think other then that, a better idea would be to turn and set absolute accuracy instead of relative.

Yep, we had that set too (in my old job, not here.)

Until there is some geometry PTC defaults the part extents to something like 1000x1000x1000.

A circle 1 inch in diameter allows the software to evaluate the extents to about 1x1x1 which, for hand-sized parts, is a good choice. Being cosmetic, it doesn't affect much else and it used to be one could not use it as the basis for any other geometry, limiting the chances for building dependencies.

It's a reasonable thing to have in the start part to force some sense of proportion/scale/extents, which is what relative accuracy is gauged against.

I would put it and any other default geometry into a group called Default_geometry, so it can be compacted at the top of the feature tree. I've seen some models where half the screen space is take in default geometry, most of which isn't used.

GrahameWard
4-Participant
(To:dschenken)

David Schenken wrote:

...

It's a reasonable thing to have in the start part to force some sense of proportion/scale/extents, which is what relative accuracy is gauged against.

...

Do you think though, that once you have started creating geometry you would no longer need that cosmetic and could delete it? I can't see how it could continue to influence the file when there are subsequent dimensioned features that are bigger.

You could delete it, mostly harmlessly. I don't believe there is any geometry/software problem caused by deleting it. If there is a process built that depends on it by name or other characteristic, you'd have to care about that.

For example - screen positioning of a model - where it shows up on the screen - is dependent on the extents of the part/assembly. If you are doing screen caps of multiple configurations where the extents are affected, this can cause the model to shift location. If the cosmetic is set to be as large as the largest extents, then the model won't shift. If that curve is part of the screen cap process, then keeping it is a good idea.

David Schenken wrote:

Until there is some geometry PTC defaults the part extents to something like 1000x1000x1000.

Is there a config setting to change this to something smaller like 50x50x50 or what ever one might designer? That should eliminate the need for a piece of geometry that will just be deleted later.

....not even a pile of foetid dingo's kidneys?? I'd actually considered doing that. And yes, I agree, that once you have actual geometry in there, you can detele it. Your coworkers are wrong, once other geometry is in there, the datums etc. scale to fit that. I don't buy the "memory" nonsense either. UNLESS it has something to do with the Relative accuracy, but I'm not even buying that. Anyone from PTC want to chime in on that?

There is actually a way to size your datums and axiis and that will drive the initial zoom, but then, the datums need to be resized, and it's more work doing all that than simply deleting one feature.

Glad you mentioned this, I was tempted to do this here.

I was thinking about this some more. Years ago I took care of this just by opening the start part, scrolling in a bunch and saving the start part and it saved the position. I have NOT tried this anytime in recent years, so I do not know if that works any more.

Only one tip if those other yahoos are no longer in the picture:

  • Make your start parts and assemblies with -sized- datum planes.

This will limit the bounding box in a similar manner as the cosmetic sketch did.

With today's relative accuracy algorithm, this -should- not be an issue.

This may have been an oversight in the Creo Elements|WF5 offering.

I believe the relative accuracy implementation will always be a problem for new users and each will come up with what they believe is the "right" Pro|WorkAround^TM.

I have not had any issues with the initial bounding box of a new and empty part or assembly.

Once the 1st feature is created, a new bounding box is created.

You can easily investigate the bounding box size; in Creo 2 - Tools tab; Investigate; Model Size.

1st thing I do in a new sketch of a new part is to draw a 1" circle. Then I proceed with my sketch and later delete the circle. I do this because I no longer use start parts.

But then those datum planes no longer automatically resize... and it's harder to unfix the size of datum planes than to delete one cosmetic sketch.

Is relative accuracy no longer dependent on bounding box diagonal length? What was the algorithm change?

It is easy to unlock the size of datum planes but yes, it is all about preference. -If- I used start parts, I would certainly lock the size to my normal expected sizes. Pretty much everything I work with fits in a shoebox. A big shoebox maybe, but certainly not a diagonal of 881.0254 inches.

I don't know what has changed since my last heavy involvement before Creo was 2000i with a brief stent with WF4. However, the relative accuracy is dependent on the current bounding box. It seems to be dynamic where only once did I have a problem with creating a first feature where the relative accuracy caused the feature creation to fail. This is the exception rather than the rule.

I find myself resizing datum planes and axes on a regular basis. All too often I have a plane stick out into no-where simply because a sketch feature exists out there.

I would much rather have a config.pro setting with initial_boundary_box 1,1,1 options. But that's not the case today.

In my experiment, this is what I ran into, I had to resize all 3 after the initial feature, and the 3 axis we use were "sized" to the datum planes so they were automatic. Seemed more trouble than simply erasing a feature. Hmmmm, maybe an annotation note might work? Maybe a datum curve put on a specific layer (not user for anything else?) in the start part and hidden right off the bat?

<sigh>

Ok, I give up - how can I resize the datums to something reasonable. When I hit the 'Refit' button, my model shrinks to a dot. I've tried selecting the randomly oversized plane, model, plane and changing the visibility, but nothing happens. Well, something does happen, but I'm ignoring the rapid rise in blood pressure and frustration.

Thanks again.

Are your datums default? Or do they come after you have created geometry? Because if they are default size they will be as big as whatever is there, even if it is hidden on a layer and you don't want to ever see it again.

They come in on iimported files and in existing models.All layers that I can unhide are unhidden.

Just curious : Does Franz Kafka work for PTC?

If you only changed the option to "size" then yes, they will still be very big. You want to also set the size to something reasonable. If your object is not created near the parts universal 0, 0, 0, then you will also get a very large field of view (extensive zooming out).

When I start a part, I create a datum coordinate system and the default 3 planes (click; click - done)

Most times I will simply start a sketch or extrude/revolve feature on a plane and start with a quick circle and size it to about what my part will be... say 1" OD. Fit the sketch normal to the screen and zoom all. Now I am ready to make my sketch and once I added some additional geometry, I can delete the temporary circle. once I complete this feature, my planes are where they need to be and zoom all give good screen coverage.

-If- I intend to wrap a sketch onto a feature, and it becomes a very wide sketch for a very small cylindrical feature, for instance, the sketch causes the one of the planes to extend far outside my part boundary. This is when I go in and size my planes beginning with the 1st which will resize to 500-someodd inches when I first redefine the feature. I go to the option and set size and type in 1 and 1, done. then I go to the second default plane and do the same, however, not this one is already scaled to the 1st plane.

So now I have planes locked at 1" about the origin and if my part becomes 2" big, so be it. I can unlock the planes if I wish, but rarely do I care.

As for subsequent planes and axes, I care much more. I like the planes and axes to work near the feature they were intended for. Excessive planes and axes are a visual obstruction! However, I rarely leave them locked to a features. I may use a feature to size these, but I switch it back to size after that.

Remember there is no -right way- to use Pro|E. This is just my preference and my way of working. There are plenty of other wasted mouse-clicks that add up in my daily work and play. Managing my part boundaries is only a minor instance of irritation... one PTC could easily fix by limiting the initial bounding size of a new part in config.pro.

Ok, so, I'm going to put into the start part a datum curve (circle) .25" in diameter, on a layer we will always hide. I picked .25 because the bounding box will always be slightly larger than the largest feature, and we have parts .25 inch or so, so this way the planes will always size to the largest dim of the created geometry, not be gigger than some invisible geometry and 4X the size of our smaller parts and screw up the zoom. I played with the idea of a parameter (INITIAL_PART_SIZE) that you change the value of when you're filling out your start parts, which would drive the value of the circle via relations, but, nah. I figure .25 will aways be about right, and for our larger parts, it'll look funny only in the very first sketch. That's a welcome tradeoff to me to not have the initial feature come in at 500" and want to extrude out to 200"! Especially since I have set my sketcher to NOT autozoom.

Have fun with that!

Frank, why not make it a cosmetic rather than a datum curve? It would serve the same purpose as a datum curve and there's no risk of it being accidentally referenced.

I have made datum planes sized before, usually referenced to some geometry, because it was a datum plane used to create a small feature and I didn't want to see the datum plane across the whole model. It seems adjusting the outline to a couple of values adds more info to the model and I try to get rid of stuff I don't need. That's why the cosmetic always bugged me, sitting there in the model tree, saying "delete me, Grahame, you know you want to..."

I generally don't use (read: hate) cosmetics, only threads. I have it named in my model tree, and on a special rules-based layer, and it seems to work fine. It REALLY helps with the first feature.....in keeping the new and (worse, ex-SW users) people from whining. My ears thank me.....

Yeah, I hear ya.....but curves are very lightweight features, and take up almost zero space. And, naming it leads to the illusion of importance, saying "Keep meeee......". But you're 100% right, once any feature is created you can delete it with no ill efect.

I think the problem is that even with fixed sized datums in your start part (mine are 12x12), when you try to create your first feature the extrude length, etc... comes in at something like 216.506 or similar. Once a feature is created, these numbers become closer to reality.

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