Dimensions in Sketches 9

[randy64]

Hello. Just wanting to get some opinions on something I've run across recently.

When updating dimensions in a sketch, I change the dimension. I do this because I like a "clean" sketch. For example, if the dimension is .50 and I'm making it .25 longer, I change the dim to .75.

I recently was working on a sketch created by a coworker. In his sketch the dimension was .50+.25. When I asked him about this, he said that that was his way of keeping track of the changes he was making. At first, this went against my instinct of having an uncluttered, clean sketch, but the more I've thought about it, it might make sense to do it that way.

Am I letting my OCD get in the way of a good technique, or is it best to leave a clean sketch as my legacy to others?

Your thoughts please.

 

[LynnB1]

For me personally, I prefer "clean" numbers like what you describe. I would rather keep track of changes in other ways (dated prints/markups, new revisions, emails, etc) that give me a clearer image of why the dimension changed.

I'm still pretty green (coming up on 3 years out of college), so I'm interested to hear other responses as well.

 

[Felix K. Holloway]

I really don't think it matters. It's just a weeny more amount of bits stored in the file. Whatever floats your boat.

To reinforce your coworkers point, at least there is a record of the change somewhere in the history IF someone HAPPENS to leave it out of a revision block or something. Having both there would at least maybe trigger a conversation vs. glancing over it for minimal changes.

Felix K. Holloway - Molded Fiber Glass Companies

 

[NutAce]

Doesn't bring any added value in my opinion. You only see the changed value. You still don't know why it has been done.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX11 / TC11

 

[cowski]

I often use this technique; I find it helpful early in the design stage when the design parameters are still being worked out and you feel that a certain change may need to be rolled back later. Of course it is most effective when the entire team at least knows of the technique, but there are ways to clue them in. When typing in an expression formula, you can add a comment by adding "//" to the formula; anything following the "//" will be kept as a comment. So when typing the formula, it may look like:

0.5 + 0.25 //added length for reasons

In the expression editor you will see "0.5 + 0.25" as the formula and "added length for reasons" in the comment column.

On a related note, you can add comments to features. In the part navigator, turn on the "comments" column. Then by selecting the feature and single clicking in the comment cell, NX will allow you to add some text. This can be useful if you are doing something that may seem strange to the next person working on the part or you just want to document why the feature is there.

www.nxjournaling.com

 

[JohnRBaker]

I've done this on occasion, usually if a sketch dimension represents the sum of several 'variables' derived from some other aspect of the design but not necessarily ones that could be directed linked. This way if any of these 'variables' change, it's easier to make the adjustment to the specific value in the sketch dimension/expression.

One thing to keep in mind which may help people look at how to leverage the unique capabilities that are available to you is to think of the dimensions as being part of the "design Intent" of your product. In this case, what I was doing was recording the "Design Intent" as a the SUM of several external parameters. Of course, if you were take this approach to it's logical conclusion, perhaps it would be better in situations like this by first creating an expression where you would capture these sets of 'variables' and then simply reference this secondary expression when creating your sketch, or for that matter, your feature parameter. Approaches like this can go a long way to capture your "Design Intent" not just for your own gratification, but for anyone who in the future may be expected to modify or update your models. Anything that can be done to leave behind an understanding of what and why something is what it is can prove to be very valuable.

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[Felix K. Holloway]

Thanks for the tips on commenting Cowski, I had no idea that was possible.

Great points John, thanks for reminding us about how expressions really would be the way to go if you were following the methodology you say. Update one, and all update accordingly. Good to see your posts again, the community just isn't the same without them.

Felix K. Holloway - Designer
Did I help you out? Add me on LinkedIn!

 

[Ehaviv]

I'm using commented like Cowski
But this way
0.75//0.50
New value//old value

 

[loki3000]

hey john, how come nx 11 can't dimension a diameter in a sketch?
also, happy retirement.

 

[JohnRBaker]

I don't know as I don't have a copy of NX.

As for my retirement, it is what it is.

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[PSI-CAD]

Hi John
How is it possible for you to live your retirement wihout a copy of NX ?
It should a gift from Siemens.

Regards
Didier Psaltopoulos

http://www.psi-cad.fr

 

[JohnRBaker]

When I retired last January (2016) I was not offered nor did I request a copy of NX (besides, there are NO Windows-based systems allowed in our house and I was never a fan of the way we implemented NX on the Mac).

Now I know it can be arranged since for several years I personally 'sponsored' (annually signed-off on) a free copy of NX for a 'retired' user who's still a frequent poster here on Eng-Tips.

However, I've had other things on my mind of late, which you can read about at:

http://www.eng-tips.com/viewthread.cfm?qid=419979

Now it hasn't all been as dark as it might sound, as I have been doing some 'restorations' between visits to the doctor and/or the hospital, as can be seen at:

http://www.eng-tips.com/viewthread.cfm?qid=408398

http://www.eng-tips.com/viewthread.cfm?qid=412462

http://www.eng-tips.com/viewthread.cfm?qid=415015

Note that I am recovering nicely and am about 1/4 of the way through a 12 week cardio-rehab regime (I go three days a week). I've even managed to lose a few pounds ;-)

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[PSI-CAD]

Hi John,

I did not read all your posts, I congratulate you for all your restoration work and wish you a good recovery

Regards
Didier Psaltopoulos

http://www.psi-cad.fr

 

[JNieman]

I do as @cowski does. It's useful to me and may be a 'tip' to someone checking up on my work to see if I accounted for something. If they see the dim is ".250 + .015 //finishing stock" they'll know I added a little extra material to be finished after assembly or something.

More importantly/frequently - it's me. I work in an environment where I'm /very/ frequently interrupted. It's me seeing if I did something. We all have our ways of keeping notes, and it adds nothing detrimental to the sketch. At least this wastes no extra paper. If you care about a sketch dim being a formula of values instead of a simple number, you care about silly things, imo. So yes, maybe it's a pseudo-OCD quirk.

It's no different than seeing someone's ridiculous amount of face-moves to add thickness, move a hole, etc. I find that abhorrent but it seems that people do that frequently. Makes the history look terrible, and is hard to keep track of. I prefer modifying the source data than using boolean operations or face-edit operations to adjust on the fly.

That may also be my own personal idiosyncrasy, though

 

[SMO]

randy64,

In case this wasn't mentioned, if you want to remove the math and only have the value shown, you can simply click the drop-down arrow, next to the formula, then select "Make Constant" at the bottom of the menu.

I usually like to clean things up too, prior to releasing parts - just to keep things clean and simple for downstream users to understand.

It's good practice to use this technique, if you want to track uncertain changes as that part is being developed, but not so much for leaving them behind for the next person to figure out (such as in your case now).

Not a huge deal, really, but just another time killer.




Regards,
SMO (NX10)

 

[loki3000]

does anyone else know (or john remembers) why can't NX dimension a diameter in a sketch?
or can it, but it's just slightly different to solidworks for example?

 

[JNieman]

I'm using NX10 and diameter is the default dimension when it applies auto dimensions to a circle. When I use 'Rapid Dimension' and pick a circle, it also defaults to being a diameteric dim.

 

[John2025]

I'm in NX11 and dimension diameters all the time, not sure why you can't.

 

[Felix K. Holloway]

loki3000,

The dimensional tool in sketch for circles and arcs (radius and diameter) is combined into one function. "Radial Dimension".

Using this function on a circle, you just change the option to "Diametral" instead of "Radial".

Why have two functions when you can do it all with one?

Felix K. Holloway - Designer - NX 9 & 11

 

[loki3000]

sorry, i meant dimensioning a rectangle against the centerline for a revolve feature (basically a pipe or a rolled ring). like this, except this is solidworks:

http://2.bp.blogspot.com/-nL3g1WoO5hE/U6U5z9f0MhI/AAAAAAAACCM/0KRst9wc-X8/s1600/103.jpg