×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Buliding Holes

Buliding Holes

Buliding Holes

(OP)
I am trying to make a counterbored hole on my part, but the only way I can activate the counterbore opition is to activate thread.

So I guess my question is can I have a non threaded counterbored hole?

RE: Buliding Holes

Yes,

When you are doing the hole feature make sure you have the thread option turned off (first of the three icons in the top RHS of the dashboard, second is c/sink, third c/bore) and the c/bore turned on. Then go to the SHAPE and unclick the Include Thread option.

Kevin Hammond

Mechanical Design Engineer
Derbyshire, UK
 

RE: Buliding Holes

(OP)
Kevin, When I start the hole tool, the only way I can see the c'bore icon is when I select the threaded option. When I do that then I see the the icon. Then I have to choose a thread style. Even after I deselect include thread icon, pro-e still displays thread call out on my part.

RE: Buliding Holes

David,

Once you have done the above, is the cosmetic thread still on the hole or not (it shouldn't be), and to clarify (this is something I haven't noticed before) in the hole feature dashboard (even when the cosmetic thread is not being displayed) the NOTE section still displays the tapping info..... As I said I have never seen this before (ie never looked in the NOTE section, and I always work with 3D notes turned off) and am very surprised at it....All I can say is that the fearture is correct, but I am damned if I know why the note isn't

Kevin Hammond

Mechanical Design Engineer
Derbyshire, UK
 

RE: Buliding Holes

David,

For some reason by default Pro/E includes tap info with a hole and you need to select the Tap Icon and then remove it to get the default note to remove the Tap info and show CLEAR for clearance hole. there are many other order of operation problems I've seen in Wildfire's dashboards. They should include a Pro/E G.P.S. like those in cars for the next release.

A Great Bit more on Hole Notes

The Pro/E default note annotation is pretty powerful if used properly. Below I have shown the Parameters used in the default Pro/E hole note and what information they provide to the note. If you change the hole definition between Blind and Thru depths, or Tap and No Tap the parameter values will change accordingly.

This is a lot of parameters to have in one place and has given me headaches on several occasions, which is why I have saved default hole notes for different types to text files. This will make using Pro/E hole notes a lot easier if you do the same.

"&PARAM_NAME"   VALUE-S


---------------------------------------------------------
"METRIC_SIZE"         6-32, 10-24 etc.
"THREAD_SERIES"    UNC, UNF, ISO
"THREAD_CLASS"    2B
"STD_HOLE_TYPE"  TAP, CLEAR
"VAR_THREAD"      #?# IF BLIND, OR " " IF THRU
"THREAD_DEPTH"   VALUE OR "THRU"
"NUMBER_SIZE"      DRILL NUMBER
"DIAMETER"             DRILL DIA.
"VAR_DEPTH"          #?# IF BLIND, OR " " IF THRU
"DRILL_DEPTH"       VALUE OR "THRU"
"PATTERN_NO"       # NUMBER OF HOLES IN PATTERN, or 1


If your Model Tree's Filter Settings include annotations then you can modify your hole note by right clicking and selecting Properties.

Or you can use the Annotations selection type to pick it from your screen you can also use Properties to modify the note.

 Hole Feature Params
The link above is a picture of the Feature Params accessed from Tools > Parameters.

If you have already started your drawing you can also Show the Note using Show/Erase and modify it in the model directly from the drawing, by selecting it and choosing
Edit > Value or using the Edit Value option on the pop-up, right click menu.

Well it's been a long day and even longer night.

Hope this helps.

Michael
noevil

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources