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’Ghost holes’ showing in drawing

E

EddyVE

New member
View attachment 1263









Hi all,
I am using WildFire 1.0 but this has been a Pro/E bug for as long as I can remember.
Unless I am doing something wrong...



I have a part with a pattern of 4 threaded holes. One hole falls
outside of the part, so naturally this hole is not visible in the part
.. Except when I make a drawing of the part. Then this hole appears as
a 'ghost hole' in the drawing.. :(


Is there a way to make this hole disappear in my drawing? (except of course by changing the pattern etc.)
See picture above.


This same thing happens when I cut away a piece of a part that has holes in it. The cut away holes show in the drawing ...


Kind regards
Eddy









Edited by: EddyVE
 
Why are you making holes where you have no material? You are seeing the surfaces created by the cosmetic thread. I think you can get rid of them in the drawing with show/erase but it would be much better to not make them in the first place.
 
My guess is that when you have created this holes (those 4 in front view), you have either create them using mirror or pattern, so you forget this one in empty space (well in model you cannot see it in shade, no hidden, hidden line, only when wireframe is on you can see this hole).
So check your model if there is hole in empty space.
 
Guys,


Yes, the 4 holes were made by using a pattern. I know one hole is falling outside the material but I did that on purpose because it was he easiest way to create the 4 holes!


I have done this before and sometimes the 'ghost hole' is visible in the drawing and sometimes it is not. I just don't know how to make it disappear in the drawing (apart from removing it entirely in the model of course..)


Kind regards
Eddy
 
Well first of all this isn't good modeling practice to leave holes in empty space, second if you want to create this holes with pattern then you got option to erase this fourth hole in empty space (assuming you got wildfire 2.0), when creating pattern.
 
WildFire 1.0

Maybe it is indeed not best practice, but it is easy, and it 'sometimes' works fine ... :(
 
Convert the pattern to a table and delete the phantom hole. I think your way "works" when you do not have cosmetic threads.
 
Dr_Gallup,



You are right! When I make the holes ordinary round holes instead of
threaded holes, the 'ghost' hole disappears in the drawing. That was
the reason it sometimes 'worked' for me.



You say "Convert the pattern to a table".

Is there a WildFire 1.0 command that does this?

Or do you mean delete the current pattern and replace it with a table pattern?



Thanks for your help!!



Kind regards

Eddy
 
I never used WF1. Someone else will have to give you the directions for WF1 if it is different. In WF2, select the pattern, RMB, select REDEFINE. In the dashboard, change the pattern type from dimension to table. It automatically creates a table with the values of the current pattern. Just delete the row from the table for the hole you don't want.
 
Dr_Gallup,

It works exactly as you described, in WF 1.0 too.
Worked like a charm!


Thanks a lot for your help !!


Kind regards
Eddy
 
in wildfire when ur definingthepattern you always can click on the black dot that shows on. that particular feature wil not be added on the pattern. i have done it even with threaded holes and they don't appear on the dwg. I know u already found the solution for ur post but just to give u another suggestion.
 
Hi Arroyopr,


That's a good tip. Thanks!
But I only managed to see the black dots when selecting the 'Fill' pattern type.
Is there also a way to use that method with the other pattern types?


Kind regards
Eddy
 
EddyVE,


In reference to dr_gallup's solution:


dr_gallup said:
I never used WF1. Someone else will have to give you the directions for WF1 if it is different. In WF2, select the pattern, RMB, select REDEFINE. In the dashboard, change the pattern type from dimension to table. It automatically creates a table with the values of the current pattern. Just delete the row from the table for the hole you don't want.
Click to expand...


Rather than deleting the pattern member row, I usually comment it out by placing "@!" (noquotemarks) in the pattern member column. This leaves the row and dimensional information in tact in case you need to add it back in later for some reason. This is nice especially when you have non-equivalent member spacing.
 
hi all


Highlight the offending hole , either from the screen or from the pattern list


in the model tree , press rh mouse button and simply HIDE the feature .


Cheers , JST



Edited by: jstanley
 
You also change the drawing view to a partial view and sketch the outline in a way that includes the part but excludes the "ghost hole". Not a good practice, but it would probably work.
 
You can also use a fill pattern in WF1 simply turn off the holes that you do not want by checking them. An open circle the hole will appear a closed one and it will not. Then all you have to do is a reference pattern for your threads.





Good Luck John
 
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