in my past experience, designers have to make a compromised when designing a component with threads.
Either they will use the cosmetic thread functionality which allow to represent the thread in 2D very quickly and efficiently but in 3D, the sruface still remain very flat.
Or 3D features could be created on the 3D models showing the thread but when comes 2D, the drawing looks very bad.... In addition creating the thread in 3D add weight to the file.
So in an assembly with many components having threads you end up with a lot of data to download/upload.
Here is a screenshot from Inventor. It is just an image on the 3D model which is automatically placed when selecting thread. It does not add any weight to the file and it is understood as thread for the 2D drawing. When vizualizing the 3D model it is obvious that we have a thread here. It helps understanding the design.
What is PTC solution as I really do not see any improvement even with Creo 3. The Intelligent Fastener seems to be only for standard hardwares.
Sorry, but I don't have a great solution for you. Personally, I always just model threads at a slightly different diameter than the rest of the shaft, and change the color. (This makes it easy to determine if you have the right grip length, by observing if the colored portion is sticking out of the hole or not.) I've never had a need to actually model threads, or show them graphically like in your image. I suppose you might be able to get a similar effect in Creo by creating a long skinny JPEG of one thread, and applying it as a repeating texture, changing the scale as needed to get the right pitch... but that seems like a lot of trouble.
You said: "the cosmetic thread functionality which allow to represent the thread in 2D very quickly and efficiently but..."
Could you explain how that works? I've never seen cosmetic threads show up on a drawing. I just ran some experiments, and all I could get was a few of the dimensions to appear. Checked layers, config settings, and drawing detail options... Online help leads me to believe this functionality may only be intended to work in section cuts, but I couldn't get that to work either.
If this did work, it might be a reason to actually use cosmetic sketches. We generally don't, as there doesn't seem much point. I'd thought it was just a poorly implemented way to hold thread metadata...
I would like to 2nd Chris's point that there is not a good solution illustrating threads in any version of Creo. This has caused issues with us in manufacturing and assembly. It is too difficult and memory intensive to model threads so we use cosmetic threads and this causes its own round of problems because you cant see the threads on interfacing parts. Not to mention the issues that cosmetic threads have in a drawing. I am familiar with inventors method of handling this and don't understand why PTC cannot implement a similar solution. What I have done in the past just to fake some threads in is to apply the image below to the threaded surface and stretch/shrink. And yes it is a PITA, and it looks like cr@p in drawings.
Summary- They're threads.....they have been around a long time.......this shouldn't be that hard.
I grew up with the Pro|E cosmetic threads and I find them very useful! They are well placed, and even properly trimmed if applied correctly. I find them useful in wireframe mode where you can easily see the mating thread and determine if you have sufficient clearance on all your fasteners. Otherwise, yes, they do show up in drawings and yes, sometimes they are a pain to manage in drawings; but that's another subject.
On the flipside, the "texture mapping" method, although perfectly reasonable beyond simply a reserved surface color, comes with a Creo shortcoming... Not the best texture mapping defaults on the planet. It all depends on how important it is.
I like real threads. As with all things Creo, specially the core version, it can be done but nothing is automatic. But I have made this simple for my purposes.
Bottom line; if I need threads, cut them in the part; If I have threads, at least back them with a cosmetic thread if not a more comprehensive hole feature. I'd like to keep my texture manipulation to a minimum. Too many lost image links for my comfort... too much file bulk to store them with the part. Curious about the GPU-cycle tax for textures and decals in a heavy session(?).
GPUs are generally designed to handle textures as these are typically used to substitute for complicated descriptions and computations of displaced surface geometry - as these shaded threads are set to do.
It looks from the OP image that they used circular ridges rather than helical threads as a short-cut.
I would probably use a spiral datum curve if I had to depict them. It is fairly light weight, includes the pitch and OD/ID, does not show through things like the 'cosmetic' thread does, and shows up in all modes. Just make 'hidden removal for datum curves' or whatever the Detail View Property checkbox is.
thank you for sharing your views and experience.
I appreciate Creo support in its own way threads and competitive CAD will do it their own way too.
I am planning to migrate Inventor users to Creo and most of them had never heard of Creo a few weeks ago. Yes that is possible.
Adoption and willingness to learn will be one of the keys of the success. Inventor being Inventor, I know Creo will be more efficient overall. This said there are areas where Inventor is stronger. Of course it all depends on to what matters. Some users will surely focus on the areas where Inventor is stronger and use that as an excuse to slow down adoption. Telling them where Creo is stronger will not help.
In addition, CAD models are not only viewed by experienced designers.I will have a bunch of people from sales for instance who will be vieweing products in 3D, maybe even taking screenshot to send to their customers. If threads are not seen in 3D,this will lead to a lot of questions. Do you imagine yourself seen, don t worry dear customer, be confident with your order, it is only Creo being a pain when comes to showing theads....
The bottom line is that it does not matter how Creo handles threads for 3D representation, 3D models (for CNC, simulation etc....) and on 2D. It just have to handle it efficiently and better than its competitors
At the moment, your comments confirm that it is not straightforward and there are big room for improvement.
I use helical sweep for major threads such as ACME threads whose representation is important from drawing point of view. For other threads I use cosmetic threads, As far as representation of the cosmetic threads in the drawing first i draw parametric sketch by using entities of cosmetic thread lines & convert its text style to hidden style if it has been shown on full view.To avoid confusion please don't forget to hide cosmetic threads in model , as cosmetic threads tends to show cross-lines in drawing when directly done by show lines function in layout. And for the dimensional details we can then add dimensions to the sketched entities.
Chris, I think what you are seeing in these comments is that there is no "right" way to deal with threads.
The problem is overhead. Real threads can bring your system to its knees in no time.
Even the futzin' with textures can take away useful time to other challenges.
I rarely worry about threads for the client unless the threads are a crucial design element.
That is to say that whoever needs to see them, will. But 99% of the audience could care less.
I download a lot of files from McMaster-Carr. They have decided that threads on screws is important because they show them on the part detail page.
When I have over 300 fasteners in a major assembly, trust me when I say that there is no room of 300 fasteners worth of threads. You can write off 20% of my productivity if I tried to make this a standard way of working.
To date, the most efficient method is to use the cosmetic threads built into Creo. For the most part, they are the least cumbersome, have intelligence, easy to see in non-shaded mode, simple to query, and they export if you want them.
Another real concern with true threads is importing them into other systems. Of all the import failures I get, true cut threads is the one thing that fails more than anything else.
As to texturing or coloring, there is no intelligence in this. Just a visual queue. Personally, I want to be able to remove all appearance changes to a part and not affect it. In this sense, I am saying that color coding or texturing threaded surfaces may be more work than it is worth.
In the past with wireframe based modelers, I always created female threads by boring the hole at the thread's minor diameter and chamfer the ends to the major diameter. You could query the larger to know what size the hole really is. I did a lot of work with PEM nuts at the time and I could model one from scratch in 2 minutes of less. So the second question you should be asking is if you want people to chamfer the lead-in to the thread. Personally I do only because it clearly shows a thread for my purposes, however, on a drawing, rather than a dashed line, you get 2 solid thick circles. Some drafting guru's wouldn't like that.
As to your true concern with reviewers on threads... I've been doing this for 35 years. Never once has someone pointed out a missing thread or interference due to a thread. True reviewers only care that fasteners don't bottom out and they are a reasonable quantity and size for the application, and that they have access to them.
Believe me when I tell you that the cosmetic threads in Creo is not foolproof without awareness. They will trip you up in conventional drawings in ways you could never have accounted for. PTC has addressed a lot of it, but some things still persist. Focusing on the drafting requirements is a good place to start when evaluating the best way to manage threads. The problem with Creo is keeping them hidden or properly shown in certain instances. There are times when you simply have to "sketch" the threads in the drawing and erase all cosmetic threads in a view. Another useful tool is that you can have layers specific to views. So you can selectively echo threads on and off by view if you remembered to segregate the threads by layers. This is a rare instance, but it happens.
Ever since they ripped the drafting boards out of our offices, it seems consensus of how to use CAD has fragmented what use to be a fairly robust standard. Today, we all make decisions based on how to best meet standards. The result I see is that we have these discussions with no real solution, simply because there isn't a prefect one and it is not the fault of the CAD system. At this point you have an opportunity to fix your standards. I recommend a reasonable committee to look at all sides of your CAD needs. All too often people with strong personalities will put a stake in the ground and the organization suffers from then on because the case was either not made or heard where some decisions can be extremely costly in the long run. If keeping it simple was a mantra for success, many CAD implementations are the poster child for what not to do.
whatever Antonius has written here is true. It is just a waste of time trying to create threads on the CAD model. It is better that we mention the same thing in the drawing rather than modeling it on the 3D model. The reason is, it is always a drawing given for manufacturing and not a 3D CAD model. Only during special application we do provide a 3D model but again with the drawing.