calculation of laser cut length of part

[ASHOK CHAUHAN]

Hai Friends;
i am designer in Reputed design Organisation
and Mostly I have deal with sheet metal part and plates so
i have to calculate the laser cutting length.
Presently I have calculate with length measuring
tool and adding the different length. I want quick solution
for that . if anybody know the solution please help me.

Ashok Chauhan
Sr. Designer
Pro-E WF-3 User

 

[design-engine]

are you looking to create a flat pattern of a sheetmetal part?

 

[dross]

I think he is wanting to find the length of the part edges to determine laser cutting time. Not sure what the solution would be though other than to measure the length of the edges.

 

[jsantangelo]

Create a Length or Distance Analysis Feature for each segment.

Then create a relation that adds all the lengths together.

<div style="margin-left: 40px;">TOTAL_LENGTH = LENGTH:FID_LENGTH_1 + LENGTH:FID_LENGTH_2 +LENGTH:FID_LENGTH_3 +LENGTH:FID_LENGTH_4
</div>
You could then create a 3D note to display the total length if you wanted too.

Here is a quick tutorial:
[url]http://santangelo-eng.com/proe_tuts/LENGTH_ANALYSIS_FEATURE. swf[/url] (5 MB)

Right click and "Save target as.." to save to your computer for later REF.




Edited by: jsantangelo

 

[perttu.korpela]

Hello Ashouk,

We have developed at Convia a custom software called Pro/BOM which can extract different kind of geometric information from solid models. It can extract number of holes, bends, cutting line length etc. from sheetmetal parts.

Software can output the information to a customized output file for whole assembly at once. Please let me know if you require more information. I can send a brochure for example to you.

Our English web pages ( www.convia.fi) are not really up to date but the software has fully English UI and messages.

Regards,
Perttu Korpela

 

[gigant]

Hello,


it is nessary to have a sheet meatl part.


Copie the following formula into TOOLS=> RELATIONS


TOTAL_LENGTH= (PRO_MP_AREA - 2 * (PRO_MP_VOLUME/smt_thickness())) / smt_thickness()


After that you get a new parameter TOTAL_LENGTH.

Andy

 

[mardeb]

Alternately you can try this:

1. 
   <LI>Choose or create an intersecting plane, parallel to the flat pattern. If you built the sheetmetal part on a plane to start with and used that plane to create the flatpattern choose that same plane.</LI>
   <LI>Create an intersection feature between the solid geometry and the intersecting plane.</LI>
   <LI>Perform a length measurement on the intersect feature. You get the total length. No math. No relations.</LI>

As a bonus you can save the measurement as a feature with a parameter, put the parameter in a note and always have it available.


-marc


View attachment 4557

 

[mardeb]

Andy,


I tried your relation and it works when I turn unit sensitivity off, but cannot get it to work with unit sensitivity turned on.


Do you know what I need to do to get the relation to work with units on?


Other than that the relation gives me exactly the same answer as the geographical method. (Always good to confirm that!)


-marc

 

[jaweijtmans]

Marc,

it is very simple.
Create a analysis feature for the model properties.
#analysis#model#mass properties.
Make sure you add this as a feature in your model tree.
Select at least the info for volume and area of the model to be created.
Then you can use the information of this feature in your realtions of the part.
Simple rewrite the realtion of Andy to corespond with your parameters of the mass properties analysis feature.

Example:
/*(for the volume calculation)
volume=volume:FID_MASS_PROP_1
/*(for the area calculation)
area=area:FID_MASS_PROP_1
/*(for the thickness of the sheetmetal part)
thickness=smt_thickness
/* the new formula of Andy then looks like this)
TOTAL = (AREA- 2 * (VOLUME/THICKNESS))/ THICKNESS

Off course you can give the parameters different names.
You could even use this for non sheetmetal parts, just need to have the thickness of your model constant and refer to this thickness by means of a parameter.

Hope this will help.

J.