How to control UNC holes in Family table?

[rudresh.hm]

Hi All,


I have family of parts having holes with different screw sizes like UNC 1-64, 2-56, 3-48 and 4-40 and so on.


Can I achieve required hole sizes just by entering one parameter/dimension in family table,anyway thread depth values can be controlled by dimensions.


plz let me know the ways of doing it. ( I am using WF2)


thanks in advance


-Rudresh

 

[rudresh.hm]

Hi All,


More than 70 people have vied this post, but no replies!!!

Now I am having one doubt, may be I have not stated my requirement properly.

Do I need to tell again, what I want in detail???


Please tell me, it is possible or not. Has any one faced this problem? Should we pass this to PTC for including this function in future releases?


Thanks


-Rudresh

 

[TonyJager]

one way of doing it is create all the holes you need in the part. then in the family table you just pick the ones you need.


Or you create the holes as cuts (not thru the hole GUI) the old fashioned way


you could drive the hole dia's and depth's via the family table. However the note is not paramtric, you would need to set it up via a relation (feature relation)and specify the call out you need/want.


You could create a relation something like: if holedia(of the particular feature)=.089 then the note=4-40 UNC.


Don't quote me on the proper syntax. I hope you get the idea.


I am using 2001 and have done that in the past

 

[rudresh.hm]

Thanks TonyJager,


These daysI wasfollowing the first methodsuggested by you. I dint like to have so many columns and say YES NO YES NO NO...........


I feel the second methodwill get me all I wanted. Thanks for the method suggested, I will look after the syntax part on my own.


May be people are interestedto knowthis, this post is viewed 100 times.I will put all the relation and note details soon.


Thanks


__Rudresh

 

[rudresh.hm]

I GOT IT

I have created a restricted value parameter by name METRIC_SIZE, which restrict the user to only select and not enter the parametervalues.


restricted value parameter definition file, list.lst will look like this


ND_ParamDefArr_K01 = {
{ Name = METRIC_SIZE
Type = string
Default = '1-64'
Enum = { '1-64', '2-56', '3-48', '4-40', '5-40', '6-32'}
}
}





and relations are written to provide tap and drill diameters.


relations:


if METRIC_SIZE=='6-32'
hole_dia = .11
thd_dia =.14
endif
/*___________
if METRIC_SIZE=='5-40'
hole_dia = .1
thd_dia =.13
endif
/*___________
if METRIC_SIZE=='4-40'
hole_dia = .09
thd_dia =.11
endif
/*___________
if METRIC_SIZE=='3-48'
hole_dia = .08
thd_dia =.1
endif
/*___________
if METRIC_SIZE=='2-56'
hole_dia = .07
thd_dia =.09
endif
/*___________
if METRIC_SIZE=='1-64'
hole_dia = .06
thd_dia =.07
endif
/*___________


finally a feature note is created which will have the text part as:


&METRIC_SIZE UNC -2B TAP &thd_dia[THREAD_DEPTH sym]&thd_len
DRILL &hole_dia [THREAD_DEPTH sym]&hole_len


this note can be called in drawing.


in family table we will have to just select the metric_size from drop down list, everything else is done at the back end.





thanks


-Rudresh