Hole Table ???

[Speedy]

I have just set up a Hole Table in a drawing. It took me a while to figure out, the need for a proper coord sys on the part etc.

Now, I want to add more holes to the table, how do I do this?

It seems that those holes that were dimensioned on the drawing prior to the formation of the table, are not recognised. Is this true?

Also how do I control which holes are added and which are omitted?

Is it possible to add holes that are formed by the extrusion function and not just those created by the HOLE function.

Any help appreciated.
Regards,
Speedy

 

[mjcole]

I've not used the Hole table functionality much but just tested it a bit. You can create your own table using the actual part dimensions for the holes ie &d## which you canm see if you use switch dims to see the Parameter Names for your shown dimensions. These will update if your holes or Extrusions change as long as you don't delete the original dims. The hole table functionality is great because if can place hole names on your drawing. You should be able to associate your own names to holes or extrusion features in your views but for the extrusions to be used you'll have to create your own table and enter the parameter text as &d##.

Unlike the hole table the Table functionality will allow you to modify the dimensions from the table itself like you can in Layout Drawings if you've used them you'll understand it pretty well.

I tried adding my own rows to the Hole Table but when it updated they got deleted if you try the Datum Axis list option it will list the X Y position but you'll have to add the diameters by using my method.

Michael

 

[Speedy]

mjcole,

Thanks for your help. That worked fine.
I also found that when I updated the Hole Table, any changes I made to it, added columns etc were deleted. I made a new regular table for the extruded holes.

A new question:

How do I find out what the Parameters inherent to a drawing are? By this I mean, say the drawing scale for example. I am setting up Part and Drawing templates at the moment, so reading this automatically would be a great help. I've tried &SCALE.

Thanks again,

Speedy

 

[3dlogix]

These are the drawing parameters (most common)as explained in PTC Help files.


&current_sheet
Displays a drawing label indicating the current sheet number.

&det_scale
Displays a drawing label indicating the scale of a detailed view. You cannot use this parameter in a drawing note. Pro/ENGINEER creates this parameter with a view and places it in notes automatically. You can modify its value, but you cannot call it out in another note.

&dtm_name
Displays datum names in a drawing note, where name is the name of a datum plane. The datum name in the note is read-only, so you cannot modify it; unlike dimensions, a datum name does not disappear from the model view if included in a note. The system encloses its name in a rectangle, as if it were a set datum.

&dwg_name
Displays a drawing label indicating the name of the drawing.

&format
Displays a drawing label indicating the format size (for example, A1, A0, A, B, and so forth).

&model_name
Displays a drawing label indicating the name of the model used for the drawing.

&scale
Displays a drawing label indicating the scale of the drawing.

&todays_date
Displays a drawing label indicating the date on which the note was created in the form dd-mm-yy (for example, 2-Jan-92). You can edit it as any other nonparametric note, using Text Line or Full Note.



If you include this symbol in a format table, the system evaluates it when it copies the format into the drawing.



To specify the initial display of the date in a drawing, use the configuration file option "todays_date_note_format."

&total_sheets
Displays a drawing label indicating the total number of sheets in the drawing.

&type
Displays a drawing label indicating the drawing model type (for example, part, assembly, etc.).

&view_name
Displays a drawing label indicating the name of the view. You cannot use this parameter in a drawing note. Pro/ENGINEER creates it with a view and places it in notes automatically. You can modify its value, but you cannot call it out in another note.

&view_scale
Displays a drawing label indicating the name of a general scaled view. You cannot use this parameter in a drawing note. Pro/ENGINEER creates it with a view and places it in notes automatically. You can modify its value, but you cannot call it out in another note.

Have fun

http://www.sprdesign.com

http://www.3dlogix.com

 

[Speedy]

3dlogix,

Thanks very much.

I was using &SCALE instead of the lower case &scale. The strange thing is that when I generated my own parameters in UPPER CASE in the part, they were read ok in the format of the drawing.

BTW I find the PTC help files very hard to use, the search function is very poor.

Cheers,
Speedy

[thumpsup2]