feature script - extrude's entities queries

tonvis · June 2018

https://cad.onshape.com/documents/48ec052b1145ddd86705ef78/w/91cdf3007cb145b3e5c7fbbf/e/305d955b8b71be5086653bad

I am trying to create a script for springs. In partstudio it works ok with changing variables.

Now working in feature script , I am not able to find the right entity-query

I need three bodies for the later helix with a different pitch.

The extrude1,extrude2 and extrude3 should go on top of each other , but now they can only start from sketch1

I have been studying all examples given in the Forum for weeks but still not solving the problem.

Also "Showcode" is not helping with this major question.

Can someone please help me out ?

Jake_Rosenfeld · June 2018

Hi @tonvis

I'm not sure I quite understand what you want, but if you want to make the first extrude off of the sketch, then then second extrude stacked on the first extrude, then the third extrude off the second extrude, you could try

var entity2_query = qCapEntity(id + "Extrude1", CapType.END, EntityType.FACE);;

This is a query for the end cap of the first extrude.

The other thing you could do is keep the profile query the same, but mess with the starting point ("second direction") of the extrude:

        extrude(context, id + "Extrude2", {
                    "bodyType" : ToolBodyType.SOLID,
                    "operationType" : NewBodyOperationType.NEW,
                    "surfaceOperationType" : NewSurfaceOperationType.NEW,
                    "entities" : entity2_query,
                    "endBound" : BoundingType.BLIND,
                    "oppositeDirection" : true,
                    "depth" : L_veer,
                    "hasSecondDirection" : true,
                    "secondDirectionBound" : SecondDirectionBoundType.BLIND,
                    "secondDirectionDepth" : L2,
                    "secondDirectionOppositeDirection" : // <----- Not actually sure if this should be true or false
                });

Let us know if that works!

owen_sparks · August 2018

Likewise

Owen S

Jake_Rosenfeld · June 2018

Hi @tonvis

I'm not sure I quite understand what you want, but if you want to make the first extrude off of the sketch, then then second extrude stacked on the first extrude, then the third extrude off the second extrude, you could try

var entity2_query = qCapEntity(id + "Extrude1", CapType.END, EntityType.FACE);;

This is a query for the end cap of the first extrude.

The other thing you could do is keep the profile query the same, but mess with the starting point ("second direction") of the extrude:

        extrude(context, id + "Extrude2", {
                    "bodyType" : ToolBodyType.SOLID,
                    "operationType" : NewBodyOperationType.NEW,
                    "surfaceOperationType" : NewSurfaceOperationType.NEW,
                    "entities" : entity2_query,
                    "endBound" : BoundingType.BLIND,
                    "oppositeDirection" : true,
                    "depth" : L_veer,
                    "hasSecondDirection" : true,
                    "secondDirectionBound" : SecondDirectionBoundType.BLIND,
                    "secondDirectionDepth" : L2,
                    "secondDirectionOppositeDirection" : // <----- Not actually sure if this should be true or false
                });

Let us know if that works!

tonvis · June 2018

Many thanks Jake for your quick reply.

It works now as I expected.

The Feature "New -Spring" is the one which I am working on to automate.

see

https://cad.onshape.com/documents/aaf33b36515d458f14979723/w/38ba0931c4383130ad547336/e/fc6a42bfd0626779db4926ee

If I go to Showcode in "New-spring " I get a good support as newcomer when converting numbers into strings

Is it possible that in future Showcode translates var TYBxWXmiEIHOwz_query; in a human code. This would help anybody working with Feature Script by lack of examples.

TYBxWXmiEIHOwz_query=qCompressed(1.0,"%B5$QueryM6S12$disambiguationDataA1M2S12$disambiguationTypeS13$ORIGINAL_DEPENDENCYS9$originalsA1C0M5Sa$entityTypeBa$EntityTypeS4$EDGESb$historyTypeS8$CREATIONSb$operationIdB2$IdA1S11.6$FJT1fGBxE99GR2X_0wireOpS9$queryTypeSd$SKETCH_ENTITYSe$sketchEntityIdSc$U8ZJsa67bK1BR4C6S4$FACER6R7S7$isStartFR8CbA1S11.9$FCoRMGdkVgYr0oS_0opExtrudeRbS8$CAP_FACE",id);
annotation { "Feature Name" : "Extrude 2" }

Regards

Ton

Jake_Rosenfeld · June 2018

Hi @tonvis

Unfortunately, even if they were not compressed, the queries that you get when you interact with the Onshape ui are nothing like the ones that you use when programming in FeatureScript. We use a number of different tricks to make downstream feature robust to upstream changes, and this ends up making ui queries pretty complicated. The `show code` panel is pretty good for seeing what the inputs to a feature look like in FeatureScript code, but for some good examples of human-readable code you could take a look through any of these public custom features:
https://www.onshape.com/features/custom-features

Or even take a look through all of the code for the built-in features in the toolbar:
https://cad.onshape.com/documents/12312312345abcabcabcdeff/w/a855e4161c814f2e9ab3698a/e/1609b2014b90745ff149a187

tonvis · June 2018

Hi Jake,

Thanks for your answer.

* In PartStudio my " NewSpring" is functioning OK with variable inputs

* see:https://cad.onshape.com/documents/aaf33b36515d458f14979723/w/38ba0931c4383130ad547336/e/92d15b1c456833375df278f5

Now I am trying to get this working as a full Featurescript Function which is not so simple! by lack of examples.

* The problem is that none of custom-features is giving an answer for my questions.

* With some help help from Onshape Forum and study Showcode in "NewSpring" , I hope that it is going to work.
* Supprisingly - using reverse engineering queries from Showcode are not giving errors , but also not solving the answer.

* I learned now that this is not the way to go.

* Will you please give me another push in the right direction with the following :
Questions ? sweptface1_query , plane_query, centersnap_query, pierce_query, edge_query?

* All by all this could be a good example helping other people who are struggling with FeatureScript

tonvis

Jake_Rosenfeld · June 2018

Hi @tonvis

Here are a couple extra resources to help you:

https://cad.onshape.com/FsDoc/library.html#qNothing - standard library documentation of all the types of queries you can use

https://cad.onshape.com/documents/12312312345abcabcabcdeff/w/a855e4161c814f2e9ab3698a/e/9fde5dffaf8d4e4c99aaa22c - source code of the file where all the queries are defined

For sweptface1_query, try using qNonCapEntity:
https://cad.onshape.com/FsDoc/library.html#qNonCapEntity-Id-EntityType

If you go and take a look at the precondition of helix, you can see which variables are required in the map and which aren't:
https://cad.onshape.com/documents/12312312345abcabcabcdeff/w/a855e4161c814f2e9ab3698a/e/a80a05e9b600481ba245f9b3

In this case, it looks like you want to be using TURNS rather than TURNS_PITCH as TURNS takes the "entities" parameter and TURNS_PITCH takes the "edges" parameter. It is worth noting that the "show code" panel will fill in every possible input to the feature, even if those inputs aren't necessarily required. By reading the source code or documentation of a FeatureScript function, you can see which inputs are required and which can be left out completely.

Feel free to continue along the current path you are going down, but if I might make a suggestion: you can skip the three initial extrudes if you use "opHelix" rather than "helix":
https://cad.onshape.com/FsDoc/library.html#opHelix-Context-Id-map

In general, we recommend that FeatureScript users use "op" functions when possible, as they generally take simple mathematical inputs rather than geometric ones. Onshape toolbar features (such as "helix") are somewhat more unwieldily to call because they are meant to take geometric selections from the user which are somewhat harder to manage from inside FeatureScript. In general, Onshape features (extrude(...), revolve(...), draft(...)) have corresponding, easier to use, documented internal operations (opExtrude(...), opRevolve(...), opDraft(...)).

By using opHelix directly you can skip the creation of any reference geometry, and define exactly the three helices you want to create.

As far as the rest of those queries go, I would avoid writing sketch code in the way that you have written it. When you are writing sketch code in FS, you do not need to use constrains or initial guesses. All the sketching calls will allow you to create your desired geometry directly:
https://cad.onshape.com/FsDoc/library.html#skPoint-Sketch-string-map

One additional suggestion, it seems like you're following the pattern:

var query = qCreatedBy(...);

someFeature(context, id + "foo", { "parameter" : qUnion([query]) });

qUnion is meant to combine an array of queries into a single query. Since `query` already is a single query, you could just provide it directly:

someFeature(context, id + "foo", { "parameter" : query });

In a related vein, "qUnion([])" is functionally equivalent to "qNothing()", and in most cases where you provide qNothing, you can probably get away with not passing that parameter at all.

Sorry if this answer was less helpful than I intended. Feel free to respond with what you are still confused about, or with any further questions.

tonvis · June 2018

Hi Jake,

Thanks for your help, I will try out your suggestions

tonvis

Jake_Rosenfeld · June 2018

@tonvis

Another resource for you. Here is our FeatureScript tutorial:
https://cad.onshape.com/FsDoc/tutorials/create-a-slot-feature.html

tonvis · June 2018

Hi Jake

Taken your suggestions , I finally got a working FeatureScript for Springs.

https://cad.onshape.com/documents/48ec052b1145ddd86705ef78/w/91cdf3007cb145b3e5c7fbbf/e/dea2176b361e81540db1a08c

My question is howto display informativ data as Total length, Outside diameter etc produced by the feature in UI form

I tried everything but only option is using UIHint which solves only one item.

May be you can give me a hint.

Best Regards

tonvis

Jake_Rosenfeld · June 2018

Hi @tonvis

read-only fillable UI parameters are something we've been thinking about internally, but don't really exist right now. I'm not sure if this is sufficient for you but you could do either of the following:

Print out the relevant information using println(). This information will be displayed in the FS console, which is available by hitting the "{✓}" button in the top right corner of your document.
Change the name of the part you create with setProperty(). You can change the name to anything you want, such as "14mm long 3mm wide spring" or something descriptive like that.

If you really want to, you can create editing logic that backfills parameters to whatever value you want, but its pretty complicated, and the user will be able to edit those fields. I can give an example of a feature that does this if you're interested in going down that path.

See next post!

Jake_Rosenfeld · June 2018

here is an example of how to make a read-only parameter filled by editing logic:
https://cad.onshape.com/documents/94dd7974241246afd953f6ee/w/14d3c2c7cd26df7a859166f7/e/8900f84e910871c575ede68a

tonvis · June 2018

Hi Jake

Thanks for your helpfull answer,

So " read-only fillable UI parametersis " are not yet possible, but I will give your options a try and will see what is best alternativ.

Regards

tonvis

Jake_Rosenfeld · June 2018

Hey @tonvis !

Sorry for the confusion. I did a strikethrough of my first post because read-only fillable UI parameters are totally possible! I just didn't realize we had already pushed that functionality. My second post is an example of how to make one!

tonvis · July 2018

Hey Jake,

Thanks for your help.

The example "editing logic" works and could be the answer , also found a good example in "Spurgear" .

I do't see any mistake in my source code but get a failure message see:

https://screenshots.firefox.com/SR25GOkhUSpUQif7/cad.onshape.com

I can't figure out what Onshape means with that, do you ?

https://cad.onshape.com/documents/48ec052b1145ddd86705ef78/w/91cdf3007cb145b3e5c7fbbf/e/305d955b8b71be5086653bad

I feel really good with Onshape !

Best regards

tonvisch

Jake_Rosenfeld · July 2018

@tonvis

I made a copy of your doc and tried out your feature, it looks like it's working fine now! Are you still experiencing this issue?

tonvis · August 2018

Hey Jake,

I found the mistake viz typing error in:

export function SpringEditing(context is Context, id is Id, oldDefinition is map, definition is map, isCreating is boolean) returns map
{     // isCreating is required in the function definition for edit logic to work when editing an existing feature
    if (oldDefinition.effectiv_windings != definition.effectiv_windings )
    {

        definition.l_Tot = definition.effectiv_windings * definition.pitch + (2 * definition.pre_windings * definition.wire_dia);

^ was a single f , but no complains from compiler

-

}

Problem solved I feel sorry to bother you

Best Regards

tonvis

^

tonvis · August 2018

Hi Jake,

The feature spring is working fine now.

At the moment I am trying to construct a model airplane which I designed in 2004 on a Mac in Vellum 2D.

Its difficult but a good learning fase. 6 August was my 80 year anniversery , still going strong !

Best Regards

tonvis

Jake_Rosenfeld · August 2018

Great stuff @tonvis !

Glad to have you as part of the community.

owen_sparks · August 2018

Likewise

Owen S

feature script - extrude's entities queries

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