topic Re: I'm trying to make a stent but creo identifies wrong sketch as a shape in 3D Part & Assembly Design

I'm trying to make a stent but creo identifies wrong sketch as a shape

철박_10230212 — Wed, 11 May 2022 04:56:00 GMT

I'm designing a simple stent but it seems that the sketch i put as a hole identifeis a shape. is there a way in creo to set which is a shape and which is a hole?

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

MartinHanak — Wed, 11 May 2022 06:54:54 GMT

Hi,

maybe your sketch is not correct -OR- is too complex.

In my test part Extrude 2 feature is set to remove material. Pink color is assigned to removed area (this meas hole).

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

pausob — Wed, 11 May 2022 09:22:54 GMT

I think the problem is in this area of your sketch:

This works:

and this does not:

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

tbraxton — Wed, 11 May 2022 12:03:20 GMT

That sketch is not a good idea in Creo Parametric. Complex sketches (too many entities) will surely cause issues with your models as you work with them. Multiple simple sketches are almost always better than one complex sketch.

The geometry shown appears that it could be patterned readily.

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

Patriot_1776 — Wed, 11 May 2022 15:08:58 GMT

Well, thank God that at least Creo isn't "identifying" as "Non-Binary"... LOL

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

kdirth — Wed, 11 May 2022 20:13:47 GMT

Interesting challenge. Here is my quick attempt at creating it with patterns.

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

Patriot_1776 — Tue, 17 May 2022 21:12:06 GMT

I tend to do complicated sketches myself, especially when I'm doing a curve in a skeleton part as a layout for all the parts in an assembly. For something like this, if this is actually what you want in a single sketch, the best thing to do is mirror the geometry. It might take several mirrors, but it does simplify things because then the only constraints you have besides the constraints for the original diamonds, are symmetric constraints. You don't have a ton of parallel, equal, perpendicular constraints etc. It helps the system out quite a bit.

If you try that, post up your experience. I'm on Creo 4, so, if you're on a higher version, I'd like to know if the sketcher behavior is the same.

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

철박_10230212 — Wed, 18 May 2022 04:03:02 GMT

I just started creo so i dont know much but ill definately try it

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

철박_10230212 — Wed, 18 May 2022 04:04:41 GMT

I'm on creo 6 and I guess it's not compatible sad...

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

철박_10230212 — Wed, 18 May 2022 04:05:29 GMT

those 2 look close but they aren't connected thx for the possible solution tho

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

철박_10230212 — Wed, 18 May 2022 04:06:15 GMT

I know this is one of the solutions but im trying to do the stent without removing the area

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

pausob — Wed, 18 May 2022 05:29:59 GMT

Well then, if they're not connected, then the area marked with "X" not "enclosed", is it?

That explains why it isn't shaded...

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

철박_10230212 — Wed, 18 May 2022 06:24:26 GMT

that's the thing i dont want the diamond shaped parts shaded i want every thing else to be

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

pausob — Wed, 18 May 2022 07:06:55 GMT

there is a somewhere in your sketch where the loop isn't closed.

This works:

and this doesn't:

Since I don't see any highlighted-in-red open endpoints, it makes me think that your sketch has a duplicate line which

overlaps another one in the boundary loop, e.g.:

Use the inspect tools to find the problem geometry:

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

kdirth — Wed, 18 May 2022 12:43:22 GMT

It is done in Creo 7.0.

I created a cylinder surface and made a feature measurement of the circumference. Then I made a relation to that measurement.

I then made a wrap feature using relations to control the width of the pattern. I sketched one pattern of diamonds with the distance between centers being the circumference divided by 2 times the number of patterns desired.

Next I trimmed the cylinder surface by each of the diamonds.

I then patterned each feature. The wrap was patterned by axis the desired number over 360 degrees. The rest of the features are then patterned by reference.

Lastly I thickened the surface.

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

Patriot_1776 — Wed, 18 May 2022 20:54:01 GMT

Ok, this was kinda interesting, the first one in a long time besides the colander (that I haven't had time to get to, so, I just spent an hour or so on it. You can modify the "OD" dimension from 1" to 3" (as shown) and it will actually make the stent shorter, which is what I believe it actually does at installation when you inflate it. The model is simple and seems pretty robust. The sketch LOOKS complicated, but as I said, using the mirrors it's actually pretty simple. It's not going to be perfect, since in Creo you can't "distort" or "stretch" material in the way it does in real life, but it should be very close. I used a midplane/neutral axis for the spinal bend so that the thicken would cut the distortion in half from that midplane on out to the outer and inner surfaces, it of course could be changed to the outer or inner dia by changing the sketcher relations etc. I also made the part flexible so that you could change the "OD" dimension at assembly and it would stretch and shorten compared to the static geometry (1" dia and 3" length). This is a Creo 4 file so pretty much everyone should be able to play with it except for "student edition" users.

Have fun y'all!

Thoughts, comments?

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

Patriot_1776 — Wed, 18 May 2022 23:12:44 GMT

Ok, since I can't edit the comment above to replace the .zip file, I'll re-do it. It turns out Creo is kinda stupid, and that vertical line in front prevents you from adding a round there, it kinds treats it as a single part, but with 2 co-planar ends. Retarded. I looked at doing a Toroidal Bend, but it failed every time. Honestly, I've NEVER had luck with that feature, dunno how it's actually used (IF it's used). So, what worked was having to add 2 extra features, splitting the quilt into 2 halves, then re-merging them, right BEFORE the thicken feature. Stoopid, but now, Creo treats it as a single continuous solid, instead of split. PTC should fix that so that if you use a spinal bend and the ends are coincident, it at least gives you the option to make it a "loop". Wheird. Hate having to add a couple of features that I would consider not needed if Creo joined the ends (like the toroidal bend that didn't work), but whatever. So, here's the new Creo file.

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

pausob — Thu, 19 May 2022 00:48:13 GMT

Nice work @Patriot_1776 Your model is very flexible - as it should be 🙂

It works well out-of-the-box and design intent is captured very well.

The split/re-merge technique to "weld" the spinally-bent surface is also a fine work-around that results in neat and tidy geometry that is easy to manipulate; for example, rounded:

Thanks for posting it. I'm adding this one to my reference library.

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

Patriot_1776 — Thu, 19 May 2022 01:08:45 GMT

Why, thank you, and glad you enjoyed it! Hopefully it can help you and/or others in the future. I was pretty annoyed that the ends of the solid didn't "merge" but, hey, I've been using the Pro/WORKAROUND module for 25+ years, so... I tried a couple different things (adding a little solid piece there in the 3 split places) that DIDN'T work, so I had to try something else. Creo REALLY struggled with that split, like it didn't know what to do. So, I figured splitting the surface and then merging it MIGHT work, and it did. I had a few other tricks up my sleeve to try if that didn't work, but I liked this a little better as it's a little cleaner. With the old PC I'm stuck with for now, I tried to add "intent edge" rounds to the 4 inside edges of the diamonds, and man, it REALLY bogged down. I figure the OP can add them if he wants. I just picked a nice round number of diamonds (X = 8, Y = 3). The same technique in the sketcher could be used for however many the user wants, the method is what matters. I could have done it in "1 diamond" segments with an axis pattern, and made a list of relations for the number of diamonds and different OD to make a full cylinder, but, this was enough to prove the point that it CAN be done.

Enjoy!

Re: I'm trying to make a stent but creo identifies wrong sketch as a shape

철박_10230212 — Fri, 20 May 2022 12:45:06 GMT

i found that i had a few overlapping lines in blue I erased and placed them again and they still turn out overlapping is there a fix to this?