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

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.

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

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