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Visualizing threads on 3D models with Creo


Visualizing threads on 3D models with Creo


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.


Best regards

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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...

5-Regular Member

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.


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.

Hello everyone

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.


Best regards

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.


Hi Chris,

      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.



Hi B M Vinay

I am afraid but I must disagree with your comment. If you want to move your company to more Part/Model centric then you must consider review and approving design without 2D drawings. I actually hoping to get the creation of 2D drawings as part of a background process ie done automatically according to the model statuses.

I have gone close to that goal in my previous company and hope to achieve it in my new company.

Strictly speaking about processes and waste removing, having a file for 3D and a file for 2D is a pure waste. Some company which have only installed 3D, still think 2D and see 3D has a nice feature but a burden and often users take short cut. Those companies who want to move to part/model centric realize that the software still has many limitation as the one which is the topic of this thread.

As a business system manager I have no preferred system. I take the requirements, evaluate, review cost (not only licences, but cost of training, migration, data model changes, etc....) and base the decision on facts. Obviously, it has been decided to move from Inventor to Creo but I know that a core of my user base will give me a hard time because of how poorly Creo handles threads compare to Inventor.  While I can argue that Inventor manages many other functionalities much less efficiently than Creo (obviously otherwise, I would have not recommended to move to Creo), I am trying to find how I can educate my new users.

In addition, as mentioned, how can we do a design review if threads are not easily readable in 3D (and easy to make)......

Thank you all for your comments. I would say that I understand that there is no efficient way to do it with Creo. This has not changed for a very long time. (I had implemented Creo (actually up to Creo Element) in the past. I see that in 3 new released of their product PTC still have not made any improvement in that area.

I wonder why.   I was in Stuttgart in November, I missed the opportunity to ask..

Happy new year 2016!!!

Just a quick anecdote...

I worked at a company that had a "we do it all in 3D" mentality. Of the 16 or so IPTs (areas within Engineering) 13 didn't make 2D drawings, 1 sometimes made drawings and 2 made drawings for every piece they created or purchased (if it wasn't a COTS item). The IPTs that never did drawings had something like 8 - 16 times the error rate than the two that used drawings. That ended up being a lot of dollars in bad parts scrapped, man-hours wasted chasing it down and correcting, meetings and the habitual jumping to conclusions and finger-pointing.

In speaking with the guy looking into this problem it was felt that people simply can't process 3D models, especially assembly interfaces, tolerance stack-ups, etc. the way they can with 2D drawings. Another part of the problem was the software, of which we simply haven't seen anything even close to on par with what is really needed. Picking through a model tree to get dimensions - or a bunch of them but only one active window at a time! - and trying to remember where they were usually just resulted in someone jotting down notes by hand on a piece of paper. Then, of course, there's the problem of getting that information out to every machine on the manufacturing floor, every vendor and the various assembly areas. The last hurdle was requiring everyone downstream to be at least capable in software able to decipher the model-centric data. Everyone can read 2D prints, not everyone can use the software.

(This isn't even going into the field where this also had to be available, quickly accessible by someone trained in the software's use, not reliant on hardware, sized appropriately for use by many at once with the ability to quickly jot down notes or clarifications from the design team.)

It was a disaster on multiple fronts.

I agree that 3D-centric seems like a great idea. I just don't see it being practical ​right now.

Wow Don.  I've heard it, I know it, and I get stuck in this argument in industry all the time.  That "paperless" myth is not for the general practitioner.  I can do CAD all day long and when I give it to a machine shop, they ask me what I really want.  And of course, I follow up with a drawing that leaves no ambiguity in any respect.

ASME Y14.41 is a great guide for "paperless" manufacturing.  There is not one local silicon forest precision machine shop that I know of that will make production parts from a 3D dataset unless you approved a prototype run documented by the shop themselves.

The inspection team is another hurdle to get around.  They want to know exactly what every tolerance is for every feature.  Somehow, they need to note which dimension they are measuring.  Yes, there are systems that will help within Creo, but when all you have is a viewer and multiple pages of information... I will bet you that the inspector now prints out 20 pieces of paper rather than the one drawing sheet.  Paperless my behind!

For those of you that remember comprehensive interconnect diagrams that would take weeks to generate.  A geo-functional diagram that determines wires; plumbing; etc.showing relations between components in your complete product.  Properly done they are masterpieces!  Today, you will find a schematic capture document that has a couple of system components per page and connector tabs from page to page where the system is strung along for 20+ pages.  There is no way anyone can read these with any real level of comprehension.  This is the same way I feel about ASME Y14.5 (drawings) as compared to ASME Y14.41 (paperless).

Hi All,

not sure if my comment mislead you.  I have never said to remove 2D drawings all together. What I was saying is to generate it automatically when the models have reached a certain state. Up to the business to decide if it is On Check In, or Released or whatever.

Even when using integrated CAM with CNC machine and measuring device that reads 3D models, most of the operators still want to see something in 2D and on a hard copy.

My point was to move away of 2D as been part of the process and have 2D as a result.

Furthermore, 3D drawings capabilities of Creo still need to improve especially for complex part. I recall starting developing methodology back in 2008 with Wildfire 3 and we gave as clearly, it was doing half the job. WF4 finally made significant improvement and I was able to release a policy to create 3D drawings that could be used for review in Creo View. Creo Element, improved the capability further, all going into the right direction

Anyway, the original topic of this post if how well Creo (as part of a business process, so meaning using Creo View too) handle threads and the conclusion is that it does not do it well. There are work around, there are best practices used on experience but Inventor (and as mentioned, I am not a strong advocate of Inventor) handle it better.

Thank you all for your contribution and feedback.

Best regards

Not misread. I know you weren't advocating for removing 2D. I just used your post as a springboard for showing some of the current pitfalls.

As for the cosmetic thread discussion, I'm guessing a lot of people would be satisfied if the cosmetic looked more like threads and less like a cylinder when viewed in profile.

I have found that in design reviews, 80% or better of the audience is not paying any attention because they do not know 3D CAD or even 2D drawings.  Only a small subset of your audience will be able to evaluate the model.  Thrust me when I tell you that threads are one of the smallest issues you can come up with.

Seriously... those that care to know about the treads only have to turn the part into wireframe or hidden line mode.  It works better than all the other methods combined in the long run (if you consider the weight of actual cut threads to great for your typical product or prohibitive due to increased export errors).  I would again highly recommend trying the cosmetic threads in a review in the way they are intended to be used.  I think you will find that they are a lot less of an issue than you want to let users convince you they are.  For Inventor and SolidWorks users, this is just "new".  For seasoned Pro|E users, why would you do it any other way.

I do not have Creo View but I suspect it will do exactly what Creo Parametric is doing when looking at those cosmetic threads.  As for exports, again, these "threads" are surface type cylinders that do export.  Again, an opportunity to query the thread interface within an assembly.  Not only that, you can attached a very comprehensive thread note to the feature which can be toggled on and off.

In my design reviews I usually got at least one yutz that wants to move everything around, resize everything, and basically try to cram 40 hours of effort into a few minutes, because he can use Visio and move a box from one spot to another and an expensive CAD system should be able to do the same. Then comes the scenes in Seven Red Lines about how they know an expert can do anything.

Been in a few of those, yes

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