reduce arrow's tail in drafting NX 7.5

[Weinstein]

Hello All,

I made a drawing and inserted a dimension in NX 7.5

on the chamfer dimension (3mm) I couldn't reduce the arrows tails, except for one side if I move the digit 3 toward the center.


thanks a lot in advance

 

[Weinstein]

Hello,

anybody can help here?

thanks.

 

[SOVAjuraj]

Hi Weinstein,
I also met the problem, that arrow tails of dimensions are long. But I don't know how to change it. I think that it is system set up - user can not change it. If I'm wrong I would also welcome some hint.

 

[jerry1423]

I looked at it, but could not figure out how to reduce that length.
Mine does not look as long as yours does, so i wonder if it's a customer default setting.
What you can do is add a gap to the end of the tail to reduce the length of it.

 

[SDETERS]

I think if you go into your File utilites and customer defaults. Select the drafting and select general there is a GD&t standard in here.

If you select the Line/arrow tab then at the very bottom there is a default for a dimension arrow out length. You can change this here.

I have not found a way to change this in the drawing.

 

[BEAEROHEAD]

Right click on the dimension. select the A under the settings tab. in the line/arrow tab, upper left corner, A and B fields are your adjustments.

 

[NutAce]

Right click on the dimension. select the A under the settings tab. in the line/arrow tab, upper left corner, A and B fields are your adjustments.

Don;t think this is what he is looking for...it will just make the arrow head longer. What Weinstein is looking for is to shorten the arrow's tail.
I haven't been able to find any option to do this in NX not even in customer defaults.

Ronald van den Broek
Mechanical Engineer
Cad Environment Coordinator
Wärtsilä, Propulsion Services
NX8.5.2 / TC9.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

 

[201181]

The only way to do it is to add a 'user defined symbol', line when making a break in a dimension line (not that I ever break dimension lines...).

On the menu select 'insert > symbol > user defined...'. In the dialogue that appears, select 'utility directory' from the 'use symbol in:' drop down menu, then in the right hand list of options, select 'gap 25'. In the middle of the dialogue, one can choose the 'define symbol size by' options. Select 'length and height' from the drop down menu, then change the length and height to a size such as 5 x 5 (this make a invisible rectangle, which will be used as your break). Now, in this order, choose the icon to the left of the four icons near the bottom (add to drafting object), now select the dimension you would like to add a break/gap to (anywhere on the dimension is fine), then press again on the same dimension where you would like to place the break (the cursor location as default will be the lower left corner of your 5 x 5 rectangle). This can be used to trim arrow lengths etc.

I know it's a long process, but it's the only way I have found to do this... (any other suggestions would be most appreciated).

 

[Weinstein]

thank you all for your help.

 

[BEAEROHEAD]

Then Right click on the dimension. select the A (style)under the settings tab. in the line/arrow tab, upper left corner, D field is your adjustment.

 

[BEAEROHEAD]

From previous see attached power point

 

[Xwheelguy]

BEAEROHEAD,

That's Stub Length, which is differnt than what the OP is asking - see his attachment. He wants to reduce the non-dimension side of a linear dimension's arrow "tail". Like shortening the left side (5 dashes) of this, if it were a linear dimension: ----->| |<---5.0

Stub length will only move the dimension (right) side closer to the extension lines (the | | pipes in the above). Create a linear dim with automatic placement and then make the Stub length shorter to see what I'm trying to describe.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[cubalibre000]

The solution is to set in the customer default and then on each template or drafting go to Tools->Drafting standard and click on 'Applay'. Starting now all dimension will use this new setting.

Thank you...

Using NX 8 and TC9.1

 

[NutAce]

The solution is to set in the customer default and then on each template or drafting go to Tools->Drafting standard and click on 'Applay'. Starting now all dimension will use this new setting.

Read the entire thread Cuba...it's not possible to change this....

Ronald van den Broek
Mechanical Engineer
Cad Environment Coordinator
Wärtsilä, Propulsion Services
NX8.5.2 / TC9.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

 

[Xwheelguy]

nutace,

I think he's referring to the default in the attached image, which might very well work depending upon permissions concerning customer defaults and use of templates as well. However, I do not think there is a setting which will change and existing dimension - one would have to delete and recreate the dimension after changing the customer defaults and restarting NX (if this, in fact, does work).

NX8_drafting_std.PNG

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[cubalibre000]

Change the single dimension no, but if you change in the customer default then reopen NX and apply the new setting via tools->drafting standard ne new dimension will have the new setting. Afetr that you can delete the dimension and add the dimension which the new setting.
I don't think your drawing has all dimension with arrow external.

Thank you...

Using NX 8 and TC9.1