Hose Length as a Parameter

[verge]

I want to add a parameter to a hose that represents its curve length. I would do this for something like a piece of angle iron by simply choosingthe length dimensionfrom within the relations dialog box. Unfortunately, I can't figure out how to introduce a "curve length" dimension intothe hose.


What procedure should I use? I want to be able to add up the lengths of all the hoses in an assembly so that we will know the total length of hose we need.

 

[sanjeevkar1]

hello verge.





i am attaching a file named curve_length. see if it is what you want.


2007-07-13_064804_curve_length.prt.rar

 

[verge]

sanjeevkar,


Thanks for the file. What you've sent me is just what I want to see as my end result. The problem is, I don't know where that "perim" dimension comes from. If I could insert that dimension, I'd be all set. How do I create a curve length dimension like that?

 

[verge]

Here's an example file of a hose that I might want an overall length for. It's not one sketch, but a series of sketches put together to make the hose. How can I attach a parameter to it that gives me the overall length of hose?


2007-07-13_100911_hose_curve_length.prt.zip

 

[vlad1979]

What I can think off right now is to create 6 analysis features for each sketch then add a relation to sum all the lengths together...


First make the analysis like below analysis / measure / at type select curve and feature then click on the first sketch in model tree, then click on add feature and give it a name say length1.


View attachment 3879


Then repeat this process until you have 6 analysis.


Then go to relations and add a relation like:


total_length=length:fid_length1+length:fid_length2+......+le ngth:fid_length6


Then you can show the length in drawing like &total_length.


This will be one method....

 

[verge]

Vlad,


Thanks for the response. Unfortunately, when I try to "add feature", I receive a message stating "the option Behavioral_Modeler has not been acquired". I guess that's a problem for me then...


I actually tried to do this the other day (I ran a forum search and ran across one of your old responses, actually!), and it didn't work then either

. Guess I shouldn't be laughing...ah heck, it's Friday, why shouldn't I laugh?

 

[vlad1979]

Yeah I guess you have the foundation license and not the flex....


Then create 6 perimeter dimensions like Sanjeevkar1 suggested.


Edit definition each sketch and select every piece of curve until you select all sketch:


View attachment 3880


then edit / convert to / perimeter and click on one dimension that you know it will always change, and that dimension will become variable (var)


View attachment 3881


do this for each sketch and then write a relation :


total_length=d20+d30+.... (switch dims and see what id's those perim dimensions have)
Edited by: vlad1979

 

[sip]

Hi


I would like to know how to get the length, width and thickness of a part to automatically update in the BOM. That would be using the dimensions of a simple plate, for instance.


Then, in sheetmetal, an analysis feature would have to be utilized for the unfolded length.


Can someone guide me through the process for both? WF3 M090


Sip

 

[verge]

Thanks Vlad, I think that's going to work. I'm working on it now.


Sip, I use a system that reads the dimensions from the part, then converts them to string to be used in my definition, i.e. "angle iron - 2x2x.25x36". It's a short "program" that you can copy and paste into your relations. This will create a parameter for each dimension you choose. The parameters and the description will update in your BOM automatically when the part is changed. All you have to do is choose the proper dimensions from your model for A1, E1, I1 and L1. You will then have parameters called width, length, height, and thickness.
<B style="mso-bidi-font-weight: normal">TO SHOW TWO DIMENSIONS:<?:namespace prefix = o ns = "urn:schemas-microsoft-comfficeffice" />[/B]

A1 =d0
B1 = FLOOR(A1)
C1 = (A1-B1)*100
IF C1 == 0
WIDTH = ITOS(B1) +".00"
ELSE
WIDTH = ITOS(B1) +"."+ ITOS(C1)
ENDIF


E1=d1
F1 = FLOOR(E1)
H1 = (E1-F1)*100
IF H1 == 0
HEIGHT = ITOS(F1) + ".00"
ELSE
HEIGHT = ITOS(F1) +"."+ ITOS(H1)
ENDIF
<B style="mso-bidi-font-weight: normal">[/B]
DESCRIPTION="PART DESCRIPTION- "+WIDTH+" X "+HEIGHT
<B style="mso-bidi-font-weight: normal">[/B]
<B style="mso-bidi-font-weight: normal">[/B]
<B style="mso-bidi-font-weight: normal">TO SHOW THREE DIMENSIONS[/B]:

A1 =d0
B1 = FLOOR(A1)
C1 = (A1-B1)*100
IF C1 == 0
WIDTH = ITOS(B1) +".00"
ELSE
WIDTH = ITOS(B1) +"."+ ITOS(C1)
ENDIF


E1=d1
F1 = FLOOR(E1)
H1 = (E1-F1)*100
IF H1 == 0
HEIGHT = ITOS(F1) + ".00"
ELSE
HEIGHT = ITOS(F1) +"."+ ITOS(H1)
ENDIF

I1=d2
J1 = FLOOR(I1)
K1 = (I1-J1)*100
IF K1 == 0
LENGTH = ITOS(J1) + ".00"
ELSE
LENGTH = ITOS(J1) +"."+ ITOS(K1)
ENDIF

DESCRIPTION=" PART DESCRIPTION - "+WIDTH+" X "+HEIGHT+" X "+LENGTH



<B style="mso-bidi-font-weight: normal">TO SHOW FOUR DIMENSIONS:[/B]
<B style="mso-bidi-font-weight: normal">[/B]
A1 =d0
B1 = FLOOR(A1)
C1 = (A1-B1)*100
IF C1 == 0
LENGTH = ITOS(B1) +".00"
ELSE
LENGTH = ITOS(B1) +"."+ ITOS(C1)
ENDIF


E1=d5
F1 = FLOOR(E1)
H1 = (E1-F1)*100
IF H1 == 0
WIDTH = ITOS(F1) + ".00"
ELSE
WIDTH = ITOS(F1) +"."+ ITOS(H1)
ENDIF

I1=d6
J1 = FLOOR(I1)
K1 = (I1-J1)*100
IF K1 == 0
HEIGHT = ITOS(J1) + ".00"
ELSE
HEIGHT = ITOS(J1) +"."+ ITOS(K1)
ENDIF

L1=d29
M1 = FLOOR(L1)
N1 = (L1-M1)*100
IF N1 == 0
THICKNESS = ITOS(M1) + ".00"
ELSE
THICKNESS = ITOS(M1) +"."+ ITOS(N1)
ENDIF

DESCRIPTION=" PART DESCRIPTION - "+THICKNESS+" X "+WIDTH+" X "+HEIGHT+" X "+LENGTH

 

[sip]

Verge,


This is great,


I hope I can get all my parts to update with this system. It happens too often that I have to blush because I failed to update the BOM after changing a part.


Sip

 

[verge]

Sip,


Glad to be of help. As many of the veterans around the forum will tell you, I ask way more questions than I answer

. I found this on the forum, and it's been really useful for us. It's nice, because the production people will automatically see a description with the correct part length, since it's taken directly from the model. It's also a good way to determine what length of angle iron (or any other item that we order in lengths rather than by the piece) we'll need total for a job. The parameters are there just waiting to be summed up!


Verge

 

[verge]

Thanks to sanjeevkar and vlad!

That's done it. Wow, it must be Friday!

 

[wsylvester]

verge....


allow_anatomic_features YES


that is in your config.pro?

 

[ReinhardN]

verge,
as a foundation user you could use the evaluate feature if you cant use perimeter dimension.
#insert
#datum
#evaluate
and use it in relations like overall_length=length:fid_measure
where measure is the evaluate feature and length the measurement.
allow_anatomic_features has to be set to YES
Be careful to mark the entire curve !!
ReinhardN

 

[ReinhardN]

sorry verge, didnt read your post entirely
there may be an option to add up a parameter in your bom.
If not, you could write a relation like
total_length=overall_length:sid_x1 + overall_length:sid_x2 + ....
where sid_x1, sid_x2, ... are the session ids of your hoses. Alternatively you could use component-ids.
ReinhardN

 

[verge]

Vlad, your technique worked nicely for my multiple sketch hoses. I found that it wouldn't work for datum curves, but Reinhard and wsylvester's suggestions worked perfectly for those!


Thanks to all

. If I lived in Germany, Nebraska or Romania I'd be buying the next round. Of course, then there's the fact that I never go out drinking anymore...ah well, can't be a rocker forever.