Relationships

[RobertLandry]

Does ST have a lack of relationships or maintaing those relationships? i have tried a number of different ways to make sure that two seemingly independent features have a relation. example i have a part with two legs that will always be the same width, however after i am done drawing there is no way for me to maintain that relationship without having more than one dimension.

please help and let me know if this is the new direction solid edge is going or if it is an error on my part.

thanks appreciate all the help i can get.

 

[Gemnoc]

Hi,

I think what you need to do is work with variables.

For something simple, you can have a formula for the second dimension that is the first dimension's variable name.

One way is to go back to your first feature's profile and double click on your first dimension: the Edit Formula Box at the left will show the variable name as "V91240". Copy it, go back to your second feature's profile, create the second dimension, close the dim tool, double click on the second dimension, and in the Formula field, paste the first dim's name. On the dimension, the digit will now show blue, while the dimension and projection lines will remain red. This will indicate that the dimension is controlled by another variable or a formula.

Another way (more so if you have more than one dimension to control) is to go through the Variables table (in the Tools tab). You can rename the variables so they are more explicit than "V4673".

I once made assemblies (stainless steel showcases) where all the parts were controlled by three variables in the assembly environment: length, width and height.

I'm not sure my explanation was clear. Let me know if you need clarification. Maybe the online help has something useful for "variables".

 

[RobertLandry]

Gemnoc,
Are you talking about in synchronous or traditional, i am very fluent at relationships in traditional, i too have made an assembly constrained and driven by only three dimensions. i used the variables tables quiet often in traditional and i am now moving to Synchronous and i am having problems with the way once you make a feature there is no way to go back to the "parent" sketch because it doesnt work like that, at least as far as i understand.

i am looking too see if i have a part in synchronous and i want two dimensions or lines to be the same length all the time no matter which one i change the other will to, can i do this?

thanks for your help

 

[Gemnoc]

Oops. Sorry for my mistake, didn't realize you were talking about the sync mode. I thought that by ST you meant the release, not the synchronous environment. I'm afraid I can't help you there, I've never used it.

 

[teebarr]

Have you tried the "Relate" command? Depending on the model it may work for you - it will keep faces coincident.
1. Select a face
2. Select "relate" from the dropdown on the floating toolbar.
3. Select the coincident relationship from the dropdown.
4. Finally, toggle the "persist" button.

You are right in saying that sketch relationships are not carried across to the model. Relationships must be applied to the model directly.
tony

 

[burhop]

Just to add to teebarr's reply, you can might also work with the PMI.

That is,

1.) Create your 3D part with two legs (they don't have to be perfect in the sketch like you might be used to in traditional).

2.) Create a driving width dimension (click the little lock icon) on each leg. In Variables, make Dim_1 equal to Dim_2

Now if you change Dim_1, Dim_2 will change to match.

 

[RobertLandry]

hey guys i think that you are both correct and i can find ways to make it work for this particular situation i am looking to see the fundamental way that they have set this up. i know that i can put and unlimited amount of dimensions and relate those dimensions using the variables relationship and this is a possible solution for me. however, with that said i am really a relationship oriented designer. i like my parts to be deteremined strongly on how they are related and i make all my sketches with the minimum amount of dimesions. i also have seen that they have a symmetry relationship that works for features that are symmetric but for parts that are not the only way to relate them is to use dimensions.

please let me know if there is some way of using the equals relationship that is persistant. i guess that is the real thing that i am looking for please let me know if you have any other suggestions. these have all been correct but i am looking for a wider use of this ability (relationship).

 

[donyoung]

attached find another solution.
To work in sync mode does require a complete different thinking.
Sync alone is hard to master but when you try to drive it in
the traditional way of modelling you will hit the wall very
soon ..

 

[teebarr]

Robert
Don has a point. Even driving models with PMI as suggested by Mark only work in the simplest of circumstances. I too like to use relationships but in ST it takes so long (the example i gave requires TWICE as many mouse clicks over trad method) as to become a totally impractical modelling methodology.

I have been using Sync for a year now and have found it great for imported parts. But EVERY time I try to model a part, I end up back in trad. Simple thing like patterning geometry suddenly becomes hard. At the current rate of development this system is probably 4years away from being a serious modelling tool - assuming it can make it at all.

I have high hopes for sync sheetmetal in ST2, and I also currently use sync for quickly developing ideas, but unless the part environment gets a serious rework it simply cannot cut it for part creation. Too much functionality missing and way too slow.

Tony

 

[RobertLandry]

Tony,
thanks that seems to be the thing that i am running into and i seem to feel the same way. i think it is more useful in changing imported parts which is great, but i feel that for creating new parts traditional is still the more powerful tool. most of my work involves sheet metal so i am eager to see what ST2 brings but i am worried that it will still fall well short of what i am doing now. majority of my work is recreation of existing parts for our manufacturability.

thanks for all the feedback appreciate all the help i have a better understanding of what my problems are.

does anyone know the release date for existing USA customers?

 

[donyoung]

> does anyone know the release date for existing USA customers?

the last information I've is: 29th of September

dy