Cannot pad sketch made from face of step file

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blazini36
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Cannot pad sketch made from face of step file

Post by blazini36 »

Not sure how I should be going about this, I've tried multiple things. I've imported a step file of a motor/gearbox. The step model I only need to use for external geometry for sketching another model. I made a copy of the step model and created a base model on the face that I need to grab external geometries from. This causes a warning that the "model is made of multiple solids and may lead to unexpected results". I can't figure out how else to get the sketcher to recognize the external geometries of this model.

I'm able to create a sketch and grab the geometries from the model. That sketch can be constrained. When I try to pad the sketch it always "fails to validate broken face". I run the "validate sketch" tool, get a couple of constraints that are bad, fix them, then get another error about pad has multiple solids. I've tried removing all external geometries once the stuff was in place and constraining it normally. I've tried copying the sketch into a new body without the dependencies of the model....just doesn't work.

I could just measure and make a sketch from scratch sure but it's alot simpler and less prone to error if I can do it this way, just not sure why I can't get away with it.
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GeneFC
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Re: Cannot pad sketch made from face of step file

Post by GeneFC »

Unless you need high precision you might consider just eye-balling a sketch to match the outline. No measurements needed.

It appears most of the object consists of straight edges in the sketch plane.

Gene
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Shalmeneser
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Re: Cannot pad sketch made from face of step file

Post by Shalmeneser »

Sketch(000) or Sketch001 are supported by BaseFeature.
So in each body, there are this BaseFeature and your new Pad.
But this, is creating 2 separates 'bodies' in the same Body, which is forbidden.

You can :
* move these sketches to 'eat' the BaseFeature
* or use ShapeBinder with the motor (->file).
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blazini36
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Re: Cannot pad sketch made from face of step file

Post by blazini36 »

GeneFC wrote: Wed Sep 15, 2021 8:17 pm Unless you need high precision you might consider just eye-balling a sketch to match the outline. No measurements needed.

It appears most of the object consists of straight edges in the sketch plane.

Gene
Yeah but that's not really the point, trying to learn the way to do this to save time in the future.
Shalmeneser wrote: Wed Sep 15, 2021 9:05 pm Sketch(000) or Sketch001 are supported by BaseFeature.
So in each body, there are this BaseFeature and your new Pad.
But this, is creating 2 separates 'bodies' in the same Body, which is forbidden.

You can :
* move these sketches to 'eat' the BaseFeature
* or use ShapeBinder with the motor (->file).
Thanks, I'll try this tomorrow. I didn't realize BaseFeature was a body
drmacro
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Re: Cannot pad sketch made from face of step file

Post by drmacro »

blazini36 wrote: Wed Sep 15, 2021 11:40 pm ...
* move these sketches to 'eat' the BaseFeature
* or use ShapeBinder with the motor (->file).
Thanks, I'll try this tomorrow. I didn't realize BaseFeature was a body
[/quote]

Techically, the Body is a container for a single solid. Each feature is a cumulative step in creating the final shape of that solid. The Basefeature is always the first lump of clay, in the Body, that is worked on by subsequent features.
Star Trek II: The Wrath of Khan: Spock: "...His pattern indicates two-dimensional thinking."
blazini36
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Re: Cannot pad sketch made from face of step file

Post by blazini36 »

drmacro wrote: Wed Sep 15, 2021 11:54 pm
Techically, the Body is a container for a single solid. Each feature is a cumulative step in creating the final shape of that solid. The Basefeature is always the first lump of clay, in the Body, that is worked on by subsequent features.
Thanks for the explanation, it's a little bit confusing because "BaseFeature" isn't generally present or at least not apparent. I can sketch, pad/pocket all day and never see "basefeature". I figured it was like a dependency on another body that doesn't have whatever native data a body created in Freecad from scratch would have
TheMarkster
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Re: Cannot pad sketch made from face of step file

Post by TheMarkster »

I would probably use the ShapeBinder. Create a new body and make it active. Select the motor in the tree view. Click the Blue ShapeBinder toolbar icon. Hide the motor. Select a face on the ShapeBinder and create a sketch. Add links to external geometry to the sketch.
chrisb
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Re: Cannot pad sketch made from face of step file

Post by chrisb »

blazini36 wrote: Thu Sep 16, 2021 1:09 am it's a little bit confusing because "BaseFeature" isn't generally present or at least not apparent.
Usually you start with an empty body and most models will start with a sketch and a Pad. Then this is your initial lump of clay.
In case of a BaseFeature you don't start at zero, but with something coming from outside of the body.
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Re: Cannot pad sketch made from face of step file

Post by thomas-neemann »

blazini36 wrote: Wed Sep 15, 2021 7:48 pm
with

https://github.com/realthunder/FreeCAD_ ... 3/releases

it is possible. is that an option for you?

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GeneFC
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Re: Cannot pad sketch made from face of step file

Post by GeneFC »

blazini36 wrote: Wed Sep 15, 2021 11:40 pm Yeah but that's not really the point, trying to learn the way to do this to save time in the future.
I guess it depends on whether you want to get the job done or learn something. Sometimes one is better than the other in terms of overall efficiency. If you are doing this routinely then learning is the obvious choice. If this is once and done forever, then just get'er done is more efficient.

Take it or leave it. Your choice. :?

Gene
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