Family table of a part-configuration

[six10]

I have a question regarding tables. Basically the tables don't work as I would like them to work. To be specific, I wonder if there is any way to set them up in the way that configurations work in SW.

Example:

I put a table driven screw with length 35mm in an assembly.  I mate the screw. For a million diffrent reasons, a lot of times I need 5 mm longer screw. So what I need to do in Creo, is delete a the 35mm screw, open (open and assemmble) my generic part and choose 40 mm long screw, and than mate the screw again.  I could just open 35 long screw, offset it 5 mm and rename it, but: i would mess my family table and i do double work again, so that kind of beats the purpose of family tables right? Why cant I choose the lenght /configuration/version (or however you wanna call it) of the screw within the part, so i would not have 'call' the screw in the assembly and re-mate it all over again?

Another example would be next: I pattern a part 5 times along a linear direction. Then i extrude a hole in the part. But I dont want the hole to be on all 5 patterned parts, i only want the extruded hole to be on first and fourth part. Is this possible without renaming the part under another name and then mating it on fisrt and fourth position?

Thank you for you help

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[MartinHanak · Accepted solution]

Hi,

solution of problem no.1:

• select 35mm screw in Model Tree, press right mouse button and use Replace command
• in Replace By section choose Family table option
• click "folder" icon, select 40mm screw and finish the replace action by clocking OK buttons

solution of problem no.2:

• create extruded hole as assembly feature
• pattern the hole
• in pattern definition exclude some instances (i.e. change black dots into white ones)

MH

[dschenken]

I think this fails if the requirement is changed to not include the first fastener, at least presuming the hole pattern is a REF PATTERN. At least in Creo 2 it did not seem possible to exclude the lead pattern member.

[dschenken]

You can use the Replace function and select 'Family Table' as the source of the replacement so you don't need to delete and reassemble. The version you want to have in your assembly must already exist in the table for it to replace the one that you start with.

Creo patterns don't have an easy function to not have the components of a pattern be different from one another. For that reason I rarely use patterns at all. One can assemble the first one and use the Repeat function to place all the others and, if required, Replace ones that I want to be different.

[six10]

Thank you for both answers, the solution for first problem works well. But for the second problem, let me elaborate:

-i have 1 part, that is patterned along an axis 180 degrees, 2 instances. For manufactoring reasons, 1 instance of the part has to have extruded font on the surface PART_1A and the second instance of the part has to have extruded font

PART_1B. So it's the same part that has different features, essentially. In this case, i If i create a family table and replace either one of the- instances by selected component / family table/, it replaces both instances of the part. Is there a solution to this?

I get the result i want if I mate the same part again (via MODEL/ASSEMBLE and choose PART_1B instance in the family table menu) and than hide one of the patterned instances, but the second mating is what i am trying to avoid.

[dschenken]

Creo Parametric Help Center To Replace Individual Pattern Members Using Family Tables

Creo Parametric Help Center  About Replacing Pattern Members by a Family Table Instance

I think this may only work with Table patterns and not Ref patterns.

This page, Creo Parametric Help Center About Assembling Components to a Pattern,  doesn't clarify if the lead pattern member can be excluded.

(thanks Jive for automatically neutering the title of the linked pages or to PTC Help for not using the help description as the window title; also interesting typo in first page's PTC page URL has "Abput")

[MartinHanak]

Hi,

I can confirm that Table pattern enables Creo user to set different family table instances for individual pattern instances. I tested it in CR2 M070.

MH

[six10]

Hello,

well i tried using table pattern. I can do it, when there is a linear direction, but how can i rotate the part with table pattern?

Usually, I create a part in top down assembly via CREATE/PART/THREE PLANES. So when i try to create a table pattern, i can only reference the distance from those planes, i cannot rotate the part.

If i go via CREATE/PART/AXIS NORMAL TO PLANE there is still no axis reference to choose from in table pattern. Any advice?

[MartinHanak]

Hi,

1. the assembly must contain axis which will be used to rotate the part (create it on assembly level)
2. assemble the part
3. in assembly create Axis pattern of the part (select axis mentioned in step 1.)
4. finish pattern
5. redefine pattern
6. change pattern type to Table
7. accept warning message and Edit table
8. add name of second instance into 3rd column in row containing 180 degrees value

You can investigate my example data created in CR2 M070.

MH

[six10]

Hello,

thank you for the answer. This works very good, except I cannot replicate 1 thing.

In your assembly you have the first instance of the table pattern as INSTANCE_1 (and not generic). When i do the table pattern, the first instance is always the generic one. I can change the name of the generic to instance 1 (first row in table pattern), but when i close the table, the first instance of the table stays generic (i know this when i click on the part in assembly area, and when i open the table pattern again). Is there a trick to this?

with other instances in table i have no problem.

[MartinHanak]

Hi,

it is simple, I assembled INSTANCE_1 (and not generic) and patterned it.

MH

[six10]

Thanks a lot for your answers, you've been very helpfull!