I would like to define a global variable in an assembly and reference it in a part (or vice versa). This seems like a simple task, but have been unable to figure out. I need to use this approach since I have a FEM application that interfaces with the assembly and can read and modify its global variables, but I need the use the value of the variable in an embedded part. I'm a newbie, so I apologise in advance if I'm asking something obvious or already posted.
Steve
Thanks, Wayne,
I've seen your description discussed before, but what I'm doing is slightly different, and I apologise for not explaining better. My global variable is not being used directly in a dimension, but rather feeds other equations in the Equations dialog box before being used in a dimension. Here are the equations in my part that I am using:
"Stenosis"= 0.3
"Base"= 2.78e-3
"D@Sketch0" = "Base" * (1 - "Stenosis" * 0)
"D@Sketch1" = "Base" * (1 - "Stenosis" * .0625)
"D@Sketch2" = "Base" * (1 - "Stenosis" * .275)
"D@Sketch3" = "Base" * (1 - "Stenosis" * .75)
"D@Sketch4" = "Base" * (1 - "Stenosis" * .9375)
"D@Sketch5" = "Base" * (1 - "Stenosis" * 1)
"D@Sketch6" = "Base" * (1 - "Stenosis" * .9375)
"D@Sketch7" = "Base" * (1 - "Stenosis" * .625)
"D@Sketch8" = "Base" * (1 - "Stenosis" * .25)
"D@Sketch9" = "Base" * (1 - "Stenosis" * .0625)
"D@Sketch10" = "Base"
What I would like to do is to move the global variable Stenosis from the part file into the assembly file. When I do this, however, it is not resolved.
Any other suggestions, or am I missing something?
Steve
Hmm, no other good ideas from here at this point. I tried a couple other thoughts and they did not work.
WT
1. I inserted an existing part into an assy.
2. I created an equation in the assy like tmp=.5 and this became my global variable.
3. I double-clicked on the inserted part and double-clicked on the dim I wanted to modify.
4. I changed the box of that dim to add an equation.
5. I made that dim = to the tmp variable.
6. Rebuild and the part changed accordingly.
This only works if the dimension is accessible without editing the component. It doesn't work for the number of instances in a linear pattern for example, since this number only shows up when you are actually editing the sketch containing the pattern.
If your assembly file is "Assembly.sldasm" then reference the global variable as "Stenosis@Assembly.sldasm"
This works, but I have found that the assembly model must open for it to resolve. This is disappointing and I wonder if that is a limitation of SolidWorks or something that could be corrected?
I agree, it is a short coming of SW. I have a DT linked to my assembly to drive the global variables in my top level assembly.
Each time the parameters are recalculated in the spreadsheet, the DT in SW has to manually opened up to update.
Whats worse, the linked DT had to be linked to an other excel work book, that has multi tabs and does advanced engineering calculations to define the global variable values (over a hundred parameters/global variables)
I have tried to link the original multi tab excel work book to SW as a DT and set the first worksheet to carry and calculate the variables.
No configuration rows, only one raw that recalculates based on the data entry fields on the adjacent works sheet. But SW didn't accept it.
So I had to create a simple DT excel worksheet that links to my advanced spreadsheets and reads the variables.
I have a question though, I wonder if someone could answer this.
Can I propagate the global variables from my top level assy to child assemblies and parts?
- Can I use the top level assy global variables in parts?
- do I have to link the same DT to each component?
- I know I can export/import Global Variables vie a .txt file but I think its medieval.
I am new to SW, have done this before in Inventor but my company is switching over from Inventor to SW.
In inventor the global variables update automatically upon pressing "save" in Excel more over there is iLogic to automate stuff (VBA code snippets) and model updates.
Thanks,
Kris
The only way to see assembly global variables in a part is to:
Are you having a problem because you are trying to edit the component "in-context" (Feature Tree is Blue)?
if the part is being edited in the assembly then you won't have access to the File Propertied/Global Variables/etc. of the assembly.
(above photo shows no access to assembly level equations because part is being edited in-context)
simply expand the feature of the part you want to "Link" and double click the Feature/Sketch that has dimension you want to control and use the "=" sign to access the drop down of Global Variable or enter an equation.
(above photo shows access to Global Variables by expanding feature tree and dbl-clicking on relevant feature/sketch)
I hope this helps.
This worked for me, thanks.
Yeah a need help in this field to, i tried everything posible so far i do not know how to use global variation from assembly in a part equation, and i have no idea how to do what Alex Sully proposed... so pleas HELP. Thanks
No what i am refering to is how to make the tree not blue, i can't seem too find a way...
Are you referring to editing a component in an assembly? 2014 SOLIDWORKS Help - Editing a Part in an Assembly. Exit from this mode in the top left of the command manager.
I have this bound to a hotkey as I tend to edit parts from the assembly level often.
You see what a am trying to do is write a global variable in an assembly wich would be controled by a custom property, and that global variable is not given to any dimension in assembly but rather just writen in equations tab, and then i want to control an in part dimension/equation, with that global variable....
My end goal is i have a Truck Panel wich has a side door on it , i have an extrude cut for the hole of the door on that panel part and i have a door part ( two separate parts) i want to link together that when i suppress the extrude cut on the panel part , that the door part suppresess as well, and i cant seem to find a way to write that equation.
Since my truck trailer assembly is rather big i am writing as many equations posible to run the given assembly ( so many Iff statements) so that i can then run the whole assembly with some basic dimensions and suppressions thru custom properties with a nice little dropdown menu on the right side made in property tab builder, and everything else would be automatic thru equations. And when i am at iff statements, i also cant seem to find a way to write a nested iff statement in equations ( an iff inside an iff ) inside Solidworks 2015. So when I saw Alex Sully's solution i tought i had a breakthru, but for me it was just a dead end. So please if someone has a solution or knows where i could find it please speak/direct me to.... Thanks in advance
Hi Vojislav
I hope this helps
To access your top level global variables, edit your part in context, open up the equations and then click the equations folder at the top of the feature tree, you will see all the assembly global variables there, just click.
a word of warning, if you have a lot of work to do in your part equations and dont want to work in context in the assembly, then add these links when you have finished (or be prepared to delete them and add in again) because solidworks very annoyingly thinks there is a syntax error and will not let you save any changes when the equations are not edited in context.
Another method that I use to bypass solidworks limitations is to create a "data exchange" sketch. This is just a series of lines with dimensions I an interested in. In the part you can make an identical sketch linked to the first and then use driven dimensions to get your data through.
re nested if's I havent had a problem, see above, but for anything complex it is very difficult and confusing to write them in the little box solidworks gives you. If you just grab all the names you want and then export the equations, you can edit them in a simple text editor (I use notedpad++) you can nest them more easily by using computer programming style formatting, and then either import or a simple copy paste.
You might find using a design table easier for what you want to achieve, I tend to avoid them if i can because they have to open up, but they are very powerful and you have access to excels mega functionality. I use them most when I want to automate the creation of multiple configurations.
Just before hitting post I reread what you wanted, I have made a simple assembly that I hope does what you want.
We have an assembly with two parts, a block and a peg.
There is a file property called hole
the peg and the hole cut in the block are suppressed when the file property is set to 1, unsupressed when set to 0
The assembly equations look like this
the part equations look like
All the best
Rob
I will give the first solution a shot. i think it actualy might work for me, as for the data exchange sketch i am trying to go around that if posible ( i tried it , it works ) , the third solution you showed with the hole and the custom property is actualy the way i achived it as well, and as for the nested IFF i dont know , iv'e tryied everything im guesing it's because it is a Solidworks 2015...
Thanks for all your help, i'l get back to you IFF i get enything working...
I'm on 2015, not sure if you mean that's why I can do it.
I'd check your syntax carefully, its so easy to miss a bracket or a comma.
Another cool thing you can do is use AND and OR. Type IIF instead of IF,,
check out the example, might be easier than nested ifs for you
edit.. you can also introduce extra variables to produce intermediate results,, this helps with complexity dramatically. If you want to keep your global variable list unclutterd use some sketch dimensions.
Hi Steven,
Let me know if this helps. I will give you an example.
I have an assembly with a gear(large gear) and a pinion(small gear). I want to make their distances based on their pitch diameters. Here is what I did:
1. Add both files to the assembly.
Mate the larger gear coincident to the origin without aligning axes
Make the front planes coincident.
2. Use a distance mate to distance both the gear centers with an arbitrary value.
Add a gear mate with an arbitrary value.
(You can add other mates as need be to align gears but as it is not the focus of this topic, I will not show that)
3. Now go to the equations in your assembly and click on manage equations
I will not select the Dimension View mode and then I can see the D1@Distance2 mate dimension and D1@GearMate2 dimension (note: these values will show something different for you)
4. Click in the value/equation box for each of those, and then in your Feature Tree, go to the equation you want to select and then click on that. Here I will make the D1@Distance2 = = ( "dp@Gear<1>.Part" + "dp@Pinion<1>.Part" ) / 2 and D1@GearMate2 = = "N@Gear<1>.Part" / "N@Pinion<1>.Part"
5. Click ok. Now as you update your part dimensions, it will auto-update the assembly dimensions as well.
Hope this helps!
Unfortunately SolidWorks has made it difficult to share variables and formulas between different parts and assemblies in an easy way. however the feature is already builtin. you just need to learn the syntax of calling a variable from a different part/assembly.
Imaging you have a mother assembly and then you want to create a new part/assembly inside. then you want to call a variable from a sibling part assembly. you can call those variables from a part sibling as :
<VariableName>@<PartName><<IncidentNumber>>.Part
and for a assembly sibling:
<VariableName>@<AssemblyName><<IncidentNumber>>.Assembly
I hope it helps.
Also, check this out:
http://www.javelin-tech.com/blog/2016/10/solidworks-configured-assembly-dimensions/
I just tried this and it worked fine.
1. I inserted an existing part into an assy.
2. I created an equation in the assy like tmp=.5 and this became my global variable.
3. I double-clicked on the inserted part and double-clicked on the dim I wanted to modify.
4. I changed the box of that dim to add an equation.
5. I made that dim = to the tmp variable.
6. Rebuild and the part changed accordingly.
WT