A few drafting questions about Solid Edge...

[JonGD]

Hi Guys,


Our D.O. have a couple of questions with respect to some issues we are having drafting in Solid Edge (V20) and I thought some of you guys may be able to help...


1) When you use the symmetric diameter (or distance between etc.) the dimensions equally space themselves from each other nicely. Going back later and adding another dimension and it stays independent of the rest. Is it possible to group new dimensions together with the old?

2) Is it possible to "snap" linear dimensions to each other so the that the arrow-heads line-up together rather than being independent (i.e. having to place them in roughly the right spot)?

3) Is there a reliable way of putting a centre-mark on a swept profile so it is actually constrained to the curve?

 

[xedu]

JonGD,

1)(*)This is a very interesting question ! And it would be terrific if whe could do it ! The same for symmetric Ø.
You can use it for Ø dimensioning but not for linear symmetric dimensions.
So the answer is no you cannot do it !

2)Yes you can snap lin. dims to each other ! Just use the grid function and all you're dims etc will snap to the grid.
Really nice, at last you can align dims!

3)I don't know. You have to ask someone else because i'am not sure of it.

BTW, Can you ask the same question (*) to GTAC or in the official newsgroup of UGS/Siemens PLM.
Or just file an E.R. for it.
I cannot do it because i'am a european SE user.
And I can only give it to my reseller

 

[JonGD]

Xedu,

Thanks for your response, ditto on the EU user problem (we're based in the UK) and our reseller is not so good with giving help (asked them a question, their response "I'll google it and have a look..."!!).

Would love to have the same assistance that US users have from Siemens but still being discriminated against (I bet the software costs less in the US too, grrrr!!)

Anyway i digress, I used inventor before coming here and liked the way that dimensions related to each other so you could create a nice neat aligned engineering drawing with a minuimum of fuss. Sadly not so with SE!!

 

[JonGD]

And hell, i've jsut thought of a 4th question...

Is there any way to make a dimension default to selecting just the end of lines rather than allowing to click on the centre all the time? It is nice to be able to select the centre when needed, but not so good when not. End up with so many dimensions quickly placed that then need to be time consumingly moved, to break them from the point they are measuring by zooming in and alt+selecting the end of the line.

 

[xedu]

JonGD,

I think you are trying to connect dimensions to endpoints,center,etc....
Just type E endpoint,C center,M midpoint...Think MICE
Yes just like autoCAD.
Just use the help function for further help.

 

[PatCouture]

For question #1 have you tried selecting a previous dimension as a starting measuring point, normally when you do this you will join the new dimension to the existing set. But I think it works only with the distance between command.

For question #2 If I understand correctly, the distance between command should do just that if you stay in the command for several dimension.

I hope it make sense.

Patrick

 

[xedu]

BTW JonGD,

I was also a Inventor user until v10.
And I' am very glad that I made the switch !
Just have some patient ! And you will love it.

 

[KENAT]

Question #4, suspend intellisketch while placing the dimension may work.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[JonGD]

Okay if using the distance between/symmetric diameter command, clicking an old dimension then adding new dimensions works fine (selects existing base point for measuring a length / centreline for diameter). However if I wanted to then add another dimension neatly in line with the first one but next to it - e.g. two consecutive lengths on a shaft these are treat independently where I would prefer them to maintain alignment to each other for neatness more than anything. Any ideas or am i just out of luck?

 

[beachcomber]

1) To add to a group of dimensions select the appropriate dim command, then one of the dims in the group, then the new dimension point.
2) To line up dimensions try the 'Line up Text' command,or use a grid.
Personally I find a quick zoom in and drag them into position works OK. SE seems to align them if they're close.
There is no way to keep them permanently aligned.
3)Can you explain exactly what you mean.
4) You don't need to select end points. Just select the line and the dim will go to the end. If you are getting mid-points just keep your cursor away from the centre of the line.

I've attached an image to clarify

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[beachcomber]

Sorry, I missed an arrow from the draft.
Try this one.

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[beachcomber]

I messed up a bit again - that's what happens when you rush things.
The note at the top right should read:

Place this dimension.
Then to add a dimension to it
click the dim tool
then click the 167 dim
then drag to indicate stack or string"

Ignore the arrow pointing to the 210 dim.

Once a dimension set is placed as stack or string, any dim added to the set will be the same type.
You can't add a string into a stack.

Sorry for any confusion !!!




bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[donyoung]

BC
[cite]
You can't add a string into a stack.
[/cite]

you can do it, see attached animated .gif

dy

 

[teebarr]

Personally, I have found snap to grid (I don't have the grid visible) the quickest. Turning on 'show alignment' can also be useful.

Tony

 

[beachcomber]

don,
The gif only shows adding a string into a string, or stack into a stack.
In my example, the 167 & 210 are stacked dims, you can't then string the 43 onto the 167 - it has to be a seperate dim.
How did you create the aninmated gif ???

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.