We have a need to model up an assembly line. We use aluminum extrustions that come in 20ft lengths. Now We can have any lengths in our models say from .5 inch to 20 feet long. We are using teamcenter. We do not want to use deformable parts due to the fact we want to call this out on the B.O.M. with the appropriate length. I do not want to have many parts of the same length with different part numbers. What would be the best way to handle this in NX and teamcenter?
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NX7.5 Extursions for Assembly line
- Thread starter SDETERS
- Start date
KhimaniMohiki
Automotive
Part families, create a part family master as a simple section extruded 1 inch for example, then create the family members by changing this expression from within the part family spreadsheet. This will create individual items in Teamcenter.
The downside to doing it this way is that the family members are only modfyable from within the family master part spreadsheet, so you might have to create all variations in known increments but this is simply a case of dragging cells in excel.
The advantage being that your designers can only pick from a predefined set of parts.
You could alternativly create a User Defined Feature for the extruded section, with rules surrounding the length increments allowable, this would also create individual part numbers in TC.
Khimani Mohiki
Design Engineer - Aston Martin
NX8.5
The downside to doing it this way is that the family members are only modfyable from within the family master part spreadsheet, so you might have to create all variations in known increments but this is simply a case of dragging cells in excel.
The advantage being that your designers can only pick from a predefined set of parts.
You could alternativly create a User Defined Feature for the extruded section, with rules surrounding the length increments allowable, this would also create individual part numbers in TC.
Khimani Mohiki
Design Engineer - Aston Martin
NX8.5
JohnRBaker
Mechanical
You could also add your profile(s) to the Reuse Library. Parts like structural members, such as angles and channels, are part of a special class of reusable parts in that while they appear to be Part Families they are in reality created using another scheme utilizing the tools of the Reuse Library itself. And there is no reason why you couldn't add your own extruded parts to this library using the same tools.
What you do is create a master part similar to what you would do if you were going to use it for a Part Family master, only the 'family' data is stored in an external spreadsheet file and that data is accessed when adding the part file to your Assembly. The parts will still come in as Components, just that they will NOT be created 'read only' meaning that you will have no problem editing these files, changing their length to the desired size and then doing a 'Save As' for each unique length. Granted, this is not all that different than simply creating a master part of some arbitrary length and then editing it's length and doing a 'Save As', but if this really is a true 'family' where while the profile is the same shape but there are different cross-sectional dimensions, you can treat it like a Part family but still get fully editable parts.
If you have't already, download and install at least one of the standard Machinery Libraries, generally based on whether you normally work in Metric or Imperial untis. Once you've done that, open the library folders to the one labeled 'Profiles' and you will find the types of files that you will need to create including the part file, the spreadsheet files and the .krx files which controls how the parts are defined and what the dialog looks like that you will see when you add one of these parts to your Assembly. You can experiment by adding some of the profiles already in the library to see how all this works. I think once you look at what's there and if you decide tha you like how the Reuse Library behaves, it won't take to much effort to create your own entries which can then be used as if they had been part of the Machinery Library all along. And if you have Teamcenter, this can all be managed for you just as if they were normal parts being created in your assemblies.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
What you do is create a master part similar to what you would do if you were going to use it for a Part Family master, only the 'family' data is stored in an external spreadsheet file and that data is accessed when adding the part file to your Assembly. The parts will still come in as Components, just that they will NOT be created 'read only' meaning that you will have no problem editing these files, changing their length to the desired size and then doing a 'Save As' for each unique length. Granted, this is not all that different than simply creating a master part of some arbitrary length and then editing it's length and doing a 'Save As', but if this really is a true 'family' where while the profile is the same shape but there are different cross-sectional dimensions, you can treat it like a Part family but still get fully editable parts.
If you have't already, download and install at least one of the standard Machinery Libraries, generally based on whether you normally work in Metric or Imperial untis. Once you've done that, open the library folders to the one labeled 'Profiles' and you will find the types of files that you will need to create including the part file, the spreadsheet files and the .krx files which controls how the parts are defined and what the dialog looks like that you will see when you add one of these parts to your Assembly. You can experiment by adding some of the profiles already in the library to see how all this works. I think once you look at what's there and if you decide tha you like how the Reuse Library behaves, it won't take to much effort to create your own entries which can then be used as if they had been part of the Machinery Library all along. And if you have Teamcenter, this can all be managed for you just as if they were normal parts being created in your assemblies.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
- Thread starter
- #4
We have only the standard Ansi inch and Ansi metric downloaded and installed at the current time. Which standard has these profiles in it? Then I can go from there. I did not know that the standard part library has standard profile cross sections. So I could just set it up just the same. When I installed the library all we where looking for was the standard bolts, nuts ETC. Thanks!
If the length is controlled by an expression, you can override the expression value in the assembly. However, this won't work so well if you need multiple different lengths in the same assembly...
Do you want/need different part numbers for each cut length used? Or do you just want to call out a "make from" part number (the P/N of the 20ft extrusion) with a cut length?
www.nxjournaling.com
Do you want/need different part numbers for each cut length used? Or do you just want to call out a "make from" part number (the P/N of the 20ft extrusion) with a cut length?
www.nxjournaling.com
JohnRBaker
Mechanical
In both the 'ANSI Inch' and 'ANSI Metric' libraries you should find a folder named 'Profile'. In them you will find some additional folders for classes of profiles, like angles, channels, etc. You could add you own folder here with just your shapes.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
- Thread starter
- #7
Yep must be blind as a bat. (Going to be hard to find these Morels that will be popping around here soon) I looked for these earlier and did not see them until know. Off to see how these interact with the assembly. Cowski I will need to have an individual p/N for each different length. A cut list if you will.
JohnRBaker
Mechanical
Morels... Exactly where do you live?
When I was a kid, we always went out and picked them every spring and while I'm not much of a mushroom fan, my father and sister would fry them in butter and eat them right out of the pan.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
When I was a kid, we always went out and picked them every spring and while I'm not much of a mushroom fan, my father and sister would fry them in butter and eat them right out of the pan.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
- Thread starter
- #9
JohnRBaker
Mechanical
Yea, I suspect that it's going to be a while before anyone is doing any mushroom hunting up in Northern Michigan (Lewiston, near Graylord - Grayling), where I grew-up.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
SDETERS said:
In that case, I second the reusable part method.
I spent ~10 years in central IL, never did pick the mushrooms though...
www.nxjournaling.com
- Thread starter
- #12
- Thread starter
- #13
Cowski said:
I am having an issue with the above comment.
I need to have multiple different lengths in the same assembly. Would I have to do a save as on each different part length?
Need some pointers here. The Profiles act the same way in the Machinery Library.
Thanks for the feedback.
Trying to add a hand here...
If you have a (1) component in multiple places, all instances will be equal unless you have a "deformable component" and all will have the same part number. ( Item ID in teamcenter)
There is a way to force a component to change the expressions ( override) when used in an assembly, but it works such that all components with the same part number will be overridden. "all components named "x" will have the length = 350 in this assembly. "
If you go the component-way, you need to either define a deformable component or have as many Item Id's as there are different lengths in the assembly.
Regards,
Tomas
If you have a (1) component in multiple places, all instances will be equal unless you have a "deformable component" and all will have the same part number. ( Item ID in teamcenter)
There is a way to force a component to change the expressions ( override) when used in an assembly, but it works such that all components with the same part number will be overridden. "all components named "x" will have the length = 350 in this assembly. "
If you go the component-way, you need to either define a deformable component or have as many Item Id's as there are different lengths in the assembly.
Regards,
Tomas
- Thread starter
- #15
Now the I got the deformable part to work. This is not to bad. What is the issue with deformable parts and the Auto B.O.M.? All of the different length parts will have the same P/N and part name. For designing assembly lines using these tekno extrustion is there any other thoughts and or suggestions. Thanks for suggestions!
TheeCircle
Civil/Environmental
I did some extrusion framing and I used the reuse library method.
I created a length expression and then used the following excel formula to drive my options.
PARAMETERS
Option p7
FIX 1,2,3,4,5,6,12,24,36,48,60,72,
VAR 1~96+1/16
I created a length expression and then used the following excel formula to drive my options.
PARAMETERS
Option p7
FIX 1,2,3,4,5,6,12,24,36,48,60,72,
VAR 1~96+1/16
Reply to Icetea:
Assume that we have an assembly which looks like this:
Assembly_1
| Component_1
and in the "component_" there is an extrusion which has the expression "p25=50"
In the assembly_1 , create an expression
component_1:
25 = 300
Then the component_1 will be forced to have the p25 = 300 as soon as it appears in the assembly. ( when both parts are open in the same session.)
When the component is open by itself, the p25 = 50.
Note that since the component will be modified by this change , if you save "all modified parts" , the component will also be saved with the new value set.
Regards,
Tomas
Assume that we have an assembly which looks like this:
Assembly_1
| Component_1
and in the "component_" there is an extrusion which has the expression "p25=50"
In the assembly_1 , create an expression
component_1:
25 = 300Then the component_1 will be forced to have the p25 = 300 as soon as it appears in the assembly. ( when both parts are open in the same session.)
When the component is open by itself, the p25 = 50.
Note that since the component will be modified by this change , if you save "all modified parts" , the component will also be saved with the new value set.
Regards,
Tomas
Icetea73,
For more info, go to the NX help file and look up "interpart expressions".
www.nxjournaling.com
For more info, go to the NX help file and look up "interpart expressions".
www.nxjournaling.com
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