Continue to Site

Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Modeling Threaded Holes/Fasteners

When modeling Male/Female Threads Do You:

  • Create Interferences Using Canned Pro-E Hole Tables

    Votes: 0 0.0%
  • Use Your Personally Created Hole Tables

    Votes: 0 0.0%
  • Model Each Location Individually

    Votes: 0 0.0%

  • Total voters
    0

wwdaugherty

New member
I am just wondering how many users are imbedding interferences in their assembly models by using the standard PTC .hol tables. Where I work, we model all threaded features at the basic diameter (male and female). This is a lot cleaner because the interface is line on line - not an interference. If you have a complex assembly with a couple hundred faseteners, that is a LOT of interferences to sort through if you use the standard PTC approach. I know there are many ways to tackle this. I even knew a guy who was modeling screw THREADS with helical sweeps !! I think the basic diameter is a lot simpler and sure regenerates faster !!
 
I agree with you, I saw I was unableto show (Show & Erase) the dimensions on drawing as thread, let say, M6 M8 aso even you have modeled a threaded hole not a simple one & a cosmetic feature. but how do you show a threaded hole on the drawing, are you making a leader with text saying "tap <dimension>", because the representation isn't according to any standard related to sections or projections. How do your workers know to thread a hole, are they just reading the text for the hole?
 
Okay, I will try to explain how we do it. We use English system of measurement, so say you have a threaded hole that is a 1/4-20 UNC-2B. The basic diameter is .250 inch (twenty threads per inch to complete the callout). The UNC is the thread profile and the 2B is the class of fit. We would model that hole as .250 diameter and within the Pro-E diameter dimension we would add text (imbed) the remaining information. On the drawing you would show the model dimension and it would look like: .250-20 UNC-2B. I have recently created some .hol files and they create the model feature and attach a 3D note with the same information.If someone pulls up the model and just measures the diameter of the cylinder they would get a value of .250 and would not necessarily know that it was a threaded feature. Our vendors are supposed to go by the drawing FIRST and inquire the model SECOND. If you pick the feature and then menu pick 'edit' the driving dimensions will show. With our new .hol files all you have to do is show 3D annotation in your environment and turn layers on and the information is there in the part models to see. Yes, there have been mistakes made when a new vendor comes on board. By not modeling the tap drill diameter you are taking a risk of that happening. When the vendors follow the information in the documents (drawings and notes) it works. And we do not intentionally model interferences, which is what this poll is trying to ask about.
 
Thank you for the information. I thought that's the way you work and I understand the reasons you take this way. I was just wondering about the avoiding the mistakes in manufacture but this is clear to me now.


Adrian
 
Threads in ProE, and holes in general, are a laugh. Holes have improved in WF, in 2001 the lack of flexibility in referencing holes to geometry is really bad. Approaching thread as a "cosmetic" feature is the base of all other things going bad. CAD-software should have a threaded hole and a threaded cylinder as a basic feature. I'm not saying CAD should produce helical cutouts, but it should build safe models. When a threaded cylinder has the nominal outer diameter and a threaded hole has the drilling diameter then the worst that can happen is the shop forgetting the thread, but it can be applied afterwards. Having both at nominal diameter you're left in a situation you can't repair when things go wrong.


If threaded cylinders and holes were a feature then software could check interference accordingly. And if it were really smart it would even show interference when the threads don't match or the thread in the hole isn't drawn deep enough.


Alex
 
Ah, Alex, I wish you worked at PTC !! I have tried asking about such things that you mentioned, but it fell on deaf ears. We are just trying to make the best of a bad situation. I agree that the most conservative approach is just what you said. When you model the tap drill diameter there is always enough material left to add threads if you miss it. We have simply stuck by a fundamental philosophy that you will find hard to argue with: "WE DO NOT INTENTIONALLY MODEL INTERFERENCES"
 
Where I work we often use more than one pitch of the same basic
diameter on the same product so it is damn important that we check we
haven't got a thread pitch mismatch. Also a machining mistake on a
machine base might cost a week and a few thousand dollars to fix.



Many of our larger thread are turned on a lathe and the profile is
exported as an IGES file. So male threads must show major diameter and
female threads must show minor diameter.



It would be real nice if the software could interpret the cosmetic
threads better but in general I find the Pro/E method of handling
threads better in several critical areas than other CAD packages I have
used.



However saying that I still regularly avoid using the canned hole
feature in favour of separate cut and cosmetic thread feature because
they are much more flexible when the going gets tough.





DB
 
Dell_Boy, it seems like in your situation that is exactly right. I am not trying to say that PTC's default approach is invalid or useless. I am just questioning the modeling of interferences being the DEFAULT mode. Just as in tolerances, you had better hope that whomever is using your files/drawings to make parts is PAYING ATTENTION !! If you have some machined part that has some critical feature and there is some chance that it will be missed, you had better COMMUNICATE !! My company builds lasers and optical systems.Tolerances matter !!


When you have a complex assembly with 250fasteners and run a global interference check, the last thing you need is page after page on meaningless interferences. Sure as anything, you are going to miss something in the noise.
 
I wish that some of my assemblies had ONLY 250 fasteners



I have a suggestion for you that may make global interference checking easier.



Have a suppressed revolved cut feature in your screw models that will
neatly remove the thread volume. Before running your global
interference, resume the cut and verify the instances.



I currently derive all my screw type fasteners as instances of a few
family parts which makes this a relatively simple task. At a previous
employer I derived ALL screws from a single part including pan head,
csk, cap screws, sems and set screws which made it exceedingly easy to
do this.





DB
 

Sponsor

Articles From 3DCAD World

Back
Top