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Configurable text item (Sticker or Padprint)
Urs_Egger_REACT
Member Posts: 100 PRO
Hi there,
I'd like to configure a product with different sticker or padprint options. The great thing is, I can also specify a surface as a part.
However when I want to use a text with different letters I get a ton of parts for each letter of the text. Unfortunately I cannot use boolean operations since the letters are not intersecting. That makes it literally inconfigurable.
Is there a way to group those surfaces to one item so I can manage each group within a configuration?
Best Answers
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jnewth
Member, OS Professional Posts: 23 PRO
There are a couple ways I can think of. You didnt specify if a composite part would do the job, but that's what I would recommend. Now: how to make different numbers of bodies all work in the same composite!
The first is to use this custom feature:
https://cad.onshape.com/documents/e2f3157a9eba6b34464401f1/v/5bbb442dbb8634fcef9693c7/e/0f7cc7c368165593e24abb3e
Take a look at "the cool way" and "the cool assembly" (save the uncool way for later).
What that feature does is create a closed composite from the bodies resulting from one or more other features (like your extrudes). So in your example, I create two extrude operations. One extrudes the word "Invariant" and the other extrudes "AAA" "BB" or "C" from the configured text. These features, then are supplied as inputs to the custom feature and it gathers up all the bodies up in to a single composite part "Composite part 1". Try it out. The number of bodies may change but the resulting composite does not. You can see in the assembly that the assembly is configured, and that the different assembly configurations reference the different configurations of the part studio. Easy peasy, keep it sleazy.
The second way is to grab my custom feature called "text".
Grab the latest version, and take a look at the examples in the doc that contains the custom feature. When the time comes to create solids, select "create composite". The feature parameters are all configurable, so you can configure the text to be whatever you want. The result will always be a single closed composite.
I think chaining the results of one operation to the input of another is a pretty great UI pattern that I would like to see more often in the standard library. Until then we just write our own.
NOTE: Just for fun, I tried to do this "the uncool way", which is:
create configured sketch,
3 different composite operations corresponding to each of the resulting body sets.
configure the part studio and configure the suppression of the composites.
Then, in the "uncool assembly", repeat the process. Insert the 3 different configs, then configure their suppression. I tried switching between them but it doesn't work. The composite body in the uncool way gets 3 different ids, so each time you switch configs in the assembly the instance reference gets broken.
Do it the cool way.
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jelte_steur814
Member Posts: 232 PRO
Awesome feature Joshua.
Greg brown also created a few simple features based on feature input to more easily take in however many parts are created by a feature.these are called "auto Boolean' and 'auto rename', i just found he also has an 'auto composite'. (I like that naming convention)
1
Answers
Text is configurable. You might need to clarify, or share your document.
Hi @Matt_Shields
Thanks. Yes agree visible configuration in a part studio is possible.
However if you look in a partslist of a configured assembly you get a ton of parts (each letter is a unique part).
I would like to configure a whole product with different colors and text, and text colors.
There are a couple ways I can think of. You didnt specify if a composite part would do the job, but that's what I would recommend. Now: how to make different numbers of bodies all work in the same composite!
The first is to use this custom feature:
https://cad.onshape.com/documents/e2f3157a9eba6b34464401f1/v/5bbb442dbb8634fcef9693c7/e/0f7cc7c368165593e24abb3e
Take a look at "the cool way" and "the cool assembly" (save the uncool way for later).
What that feature does is create a closed composite from the bodies resulting from one or more other features (like your extrudes). So in your example, I create two extrude operations. One extrudes the word "Invariant" and the other extrudes "AAA" "BB" or "C" from the configured text. These features, then are supplied as inputs to the custom feature and it gathers up all the bodies up in to a single composite part "Composite part 1". Try it out. The number of bodies may change but the resulting composite does not. You can see in the assembly that the assembly is configured, and that the different assembly configurations reference the different configurations of the part studio. Easy peasy, keep it sleazy.
The second way is to grab my custom feature called "text".
Grab the latest version, and take a look at the examples in the doc that contains the custom feature. When the time comes to create solids, select "create composite". The feature parameters are all configurable, so you can configure the text to be whatever you want. The result will always be a single closed composite.
I think chaining the results of one operation to the input of another is a pretty great UI pattern that I would like to see more often in the standard library. Until then we just write our own.
NOTE: Just for fun, I tried to do this "the uncool way", which is:
create configured sketch,
3 different composite operations corresponding to each of the resulting body sets.
configure the part studio and configure the suppression of the composites.
Then, in the "uncool assembly", repeat the process. Insert the 3 different configs, then configure their suppression. I tried switching between them but it doesn't work. The composite body in the uncool way gets 3 different ids, so each time you switch configs in the assembly the instance reference gets broken.
Do it the cool way.
Awesome feature Joshua.
Greg brown also created a few simple features based on feature input to more easily take in however many parts are created by a feature.
these are called "auto Boolean' and 'auto rename', i just found he also has an 'auto composite'. (I like that naming convention)
https://cad.onshape.com/documents/20afd0071b1fd882855e31f3/v/a861552f5b8dcff963345bfe/e/f8364fc6d155c4ffc25d84ea
@jnewth what a gift to have featurescript and such an amazing community. Amazing! Thanks a lot.
For my specific usecase the uncool way did the job already. Did not have composite feature in mind before.
But I already have things in mind how to use the featurescript too.
@jelte_steur814 You are correct - @GregBrown told me about his auto-boolean features but I couldn’t remember the names so just hacked my own! Onshape is fortunate to have Greg running Product because he really “gets” it: what the community needs and what the tools can do.
@Urs_Egger_REACT I should not be so silly with my names. The “uncool” way totally works and I’m glad you figured out a way forward. I think the increased effort required to configure suppression and manage multiple instances on the assembly side is not as elegant to use — but it works and that’s the important part!