dimension for mirror hole

[s_pme20]

I have two symmetric threaded holes on part.I want to use hole feature to create one hole and mirror other one.Problem is: I want to have dim. between holes instead of dim. from mirror plane.and that dim. will be used in family table...i dont find a way to do that...plz help..
I want red dim. on model, to use in fam. table-->

View attachment 5353

Using WF 4

 

[SRINIVASANIYER1]

Sachin,
There are two aspects... One your design intent. i.e. you
wish to have the holes to maintain positional symmetry;
second you wish to provide for dimension between the two
holes for the purpose of a family table.
If you wish to maintain the design intent, you can add the
dimension of the hole from the plane. This should serve
your purpose.

 

[dr_gallup]

I would pattern the hole rather than mirror it. Then you will have the value for use in the family table. You can write a relation to make the initial hole location half the pattern dimension. I have always found the mirror command more trouble than it's worth except for mirroring entire part geometries where it saves remaking many features. Mirror features have soooooooo many limitations.

 

[s_pme20]

Srini, Problem is due to design intent only...there are some toletances associated so that i can not change dim. scheme...

I will try suggestions by Dr_gallup..

Thanks to both

 

[michaelpaul]

silly question, but why not just make an extrude cut and place both circles in the sketch at the same time. dimension as you want from hole center to hole center.

granted, it's not using the hole command but it solves the dimensioning problem

 

[s_pme20]

it is possible...but these are threaded blind holes(with 118 degree drill point). and i want them to be created using hole feature to avoid multiple features in tree..

 

[tobbo]

ignore the "dont want multiple features thinking". make you model as robust as you can instead!


What you could do, is to do as michaelpaul suggests, but make the extruded holes rather small.... then place your 2 Holefeatures using the axis made from the extrudes. this is NOT a perfect way of doing it , but you get the distans/dimension as you want , and you can put it in your fam table.


//Tobias

 

[s_pme20]

I should say "to avoid unnecessary multiple features" in my previous post.....
I found now multiple ways doing that, after all replies.....but i was thinking of best way..

 

[SRINIVASANIYER1]

Here is another way that would satisfy the conditions...


Sketch symmetrical points with a symmetric constraint.


Create holes with axis passing through the points. You can thus have both symmetry and the dimension between the holes (coming from the sketched points)

 

[s_pme20]

just like said by tobias...but you eliminated small holes...
what i preferred to choose is:
--> created hole-1 using dim. d33 & d34.
--> created hole-2 using dim. G & d35.
--> in part relations i have mentioned:
d33=G/2
d34=d35
so, ultimately two holes are governed by two dim. only, keeping symmetry and no exrta features.

View attachment 5355


thanks to all for ideas...

 

[dr_gallup]

Now you have two holes with symmetrical position but independent size, depth, etc. So if you change one you have to remember to change the other or write additional relations to keep them the same. If you had patterned them you they would always stay the same.