Adding Holes To An Existing Hole Dimension Table

[TorsionalStress]

Using Catia V5R18;

I created a “Hole Dimension Table” for multiple holes in a plate. I would like to know how to add forgotten or added holes to the existing “Hole Dimension Table”?

Any response will be greatly appreciated!

 

[HGMorgan]

You either have to start over, or, you can edit the table.
Edit the table to extend rows as needed.
Make a new table of just the holes added or missed.
Cut & paste from new table to modifed old table.

A CATIA V5 Table doesn't update.
One of the pains of a table is that if some holes are moved, the table doesn't update for the new locations.


Harold G. Morgan
CATIA, QA, CNC & CMM Programmer

 

[TorsionalStress]

Harold, you just shot my plane down! I have 500 holes in one plate, some with multiple hole features at the same location. Does Catia offer another way to dimension these holes?

 

[HGMorgan]

CATIA did the shooting
With that many holes, a table is the way to go, if the holes have to be fully dimensioned.
Are the holes in a pattern such that limited dim could be used? I.E.; 1st hole is .xxx .yyy from datums or edge of plate, all other holes are .xxx .yyy from each other.
Also, consider calling holes out to be per model.
Yesterday, I CNC programmed a plate with 209 ea .500 dia holes and 612 ea 1/4-20 threaded holes. I just pulled in the model and drove them. That's what CAD/CAM is for!

IF you have to fully dim all 500 ea holes:
1. Use group select to select all the holes (don't worry if other type geometry gets picked, hole table will only do circles & arcs).
2. De-select any circle geometry not desired.
3. Run Hole Table
Problem with this method is:
1. Holes ID will not be sequencial.
2. If there are a lot of multiple hole features it will still be a pain to pick the holes.

One last item: always make sure to set font size & .xxxx decimal place before pushing OK and creating table.

Harold G. Morgan
CATIA, QA, CNC & CMM Programmer

 

[TorsionalStress]

LOL! I guess your right about the shooting!
All of the holes would be referenced from the center of my round plate & not to each other.
I must confess, I have only been using Catia for 1 month now & I’ve got this mammoth project to deal with.

From your experience, would you consider ordinate dimensioning or stick with hole table even if it doesn’t update?

 

[HGMorgan]

Hole table is faster to create & easier to read for you and anybody that works with the drawing. Also, you can create separate hole tables for different hole types, I.E.; .500 Dia hole table, 1/4-20 thread table, 3/8 hole with C'bore, etc.
Try doing 10 ea holes both ways and see what you think.
Ordinate or linear dim means you have to pick each hole twice, and then dwg user has to find and correctly tie together both dim's. A table means you pick the hole once and get both coordinates together.
Ordinate or linear dim's will update upon hole movement, but not for new or deleted holes. Hole table doesn't update.
I would also look at hole pattern grouping. You could use detail view & hole table with that.
I would still strongly suggest looking for some kind of pattern. If that isn't there, then I would call out that the hole locations are per model and supply hole info and tolerances.
Good luck!

Harold G. Morgan
CATIA, QA, CNC & CMM Programmer

 

[TorsionalStress]

Harold, Thanks for the advice! I will try a couple of ways before I determine which option I will choose. In doing so, I would like to window select the view, but have Catia choose only the text features next to the holes so they can be deleted, How can this be done without individual selection?

 

[HGMorgan]

A couple of ways....

1. The Trap Selection is defaulted to select everything completely enclosed in the window...so, if you had a row of holes with text @ say upper L/H quadrant, you could window trap the text complete but not the holes, and only the text would be selected. There is a down arrow on the Select Cursor Icon that allows selection of different trap methods. One that I have found useful is the "free hand" tool, you draw a polyline thru all the elements desired and it selects them. Try that, it is useful.

2. Hide all views except for desired modify view. Ctrl-F. Hold down Ctrl key & press F key (for find) and the Search Menu comes up. In the "Type" field (Type is on top of R/H field) use down button to select "From Element". Select a text feature, then pick "Search & Select" Icon (binoculars with arrow). All text in drawing will be selected. De-select any text to be saved, and hit delete.

Gone.

Harold G. Morgan
CATIA, QA, CNC & CMM Programmer