Modify circular hole pattern diameter in syncronous 2

[Javiduc]

Is that posible?

I mean, I have imported a part with 6 holes placed in a circular pattern and separated 60º. I want to mantain these holes but move them so the circular pattern is bigger. I have tried with syncronous but I can't do it. I can delete and do them again but some assembly restrictions will be lost.

 

[cowski]

I don't think it can be done in one fell swoop (within a single command), but you could move each hole in the radial direction by the desired amount.

www.nxjournaling.com

 

[Javiduc]

Thank you, Cowski. I think is a good solution for a 6 holes pattern, I will use your advise. It would be great if syncronous could do it in one single step for patterns with more than 6 holes. Maybe in future...

 

[cowski]

It would be great if syncronous could do it in one single step for patterns with more than 6 holes. Maybe in future...

Contact GTAC and suggest this feature as an enhancement request, otherwise it will not get their consideration.

www.nxjournaling.com

 

[Toost]

i think i have seen this in Solid Edge, if that is of any help. ( for - the Enhancement Request

Regards,
Tomas

 

[SDETERS]

Could you sketch a bigger bolt circle. Apply points where you want them, and move the circular face from point to point. Then you have it where it could be changed with a dimension easily.

 

[jerry1423]

I submitted an enhancement request a log time ago for this, but the more requests they get for something the more it gets their attention.

 

[capnhook]

I submitted an enhancement request a log time ago for this, but the more requests they get for something the more it gets their attention. forgotten.

Fixed that for you jerry1423.

Proud Member of the Reality-Based Community..

[green]To the Toolmaker, your nice little cartoon drawing of your glass looks cool, but your solid model sucks. Do you want me to fix it, or are you going to take all week to get it back to me so I can get some work done?[/green]

 

[jerry1423]

well . . . I hope not.

 

[Toost]

Siemens never forgets but they are a bit slow.
Do You remember when NX got Limits & Fits tolerances ?
It was introduced in NX7.5, released spring 2010.
I wrote an ER on Limits and Fits tolerances back in 1992.

Regards,
Tomas

 

[MFDO]

That is why it feels like going back to stone age when you switch to NX.

Michael Fernando (CSWE)

http://www.solidCADworks.com

Tool and Die Designer
Siemens NX V10.0 + PDW
SWX 2013 SP3.0 X64
PDMWorks 2013
Logopress3
FastForm Advance
FormatWorks

 

[eirik]

I tried in NX11 now, and I got it to work, so maybe it will work in whatever version you are on.
First i created a hole, then i created a circular pattern (variational) of the hole, then used "move face" to move the original hole away from center of the circular pattern, then i drag-and-dropped the "move face" feature above the pattern in the part navigator, then i edited the pattern to include not just the hole, but "hole" and "move face" (two features patterned). it worked no problem.
The only "fix" detail here is that the pattern needs to be "variational method" in order to select both the hole-feature and the child, "move face"-feature.

Regards, Eirik

 

[Javiduc]

Thank you Eirik. My problem is that the holes are already created because I imported the part from an step file. So there is no feature I can modify.

 

[Arbuckle04]

One way to do this is listed below.

Do a group face on each hole, the example I worked though had counter bore holes. So I ended up with a group for each hole, in your case that would be 6 features.

Create a variable called NewDiameter and set it to the value for your new bolt pattern.

Do a move face for each group of faces use the radial distance type, set the value to NewDiameter/2. In your case this would need to be done 6 times.

You now have a solution and can update the bolt circle diameter.

If you need to change the clocking you can also add 1 more move face using the Angle type, for the selection step pick all of your face groups.

Hope this helps.
Scott

 

[Ehaviv]

Here is an example using pull face and a distance expresion (new_dist)
now its a parametric and can be changed as required.

 

[Ehaviv]

added case of original distance

 

[Ehaviv]

In a simple way ( with sketch patterns and pull face )