How to edit a Stepfile - something strange

[meme2704]

I believe that you use V0.16, in this version, every time you do 1 operation on 1 colored object, it returns to the color by default

[White_Fox]

Thanks...step by step I get FreeCAD under control.

But there is one other...how could I slice the step model? To remove the single pin was'nt a problem. I've found the slice-tool in part workbench, but it seems not working like I use it.

Edit: Now I work with v0.17.

[GeneFC]

This is one case where remaining with version 0.16 is OK.

* Import the Step file into a new document.

* Switch to Part WB if not already there.

* Fuse all five features of the Step file.

* Create a Box and position it as wanted over the legs of the device.

* Perform a Boolean Cut of the Box from the Fusion.

* Legs are cut off and the color remains.

This should also work in 0.17, but I did not try it.

Gene

[easyw-fc]

This is one case where remaining with version 0.16 is OK.

....

This should also work in 0.17, but I did not try it.

Gene

All which is working in Part WB in FC0.16 can be done in Part WB in FC0.17, so no need to stay in FC0.16

FC0.17 has the new Part Design WB, but this is all a new workflow

Moreover FC0.17 is going to be released as the new stable, so FC0.16 will be no more supported...

The doc I posted above can be opened in FC0.17 and used there without any issue (I just did some boolean ops in Part WB)

[White_Fox]

Ok...it works well, more and more. Old pins are removed.
Now I wanna add new pins. Is there any way to get some anchorpoints to get position and diameter in a sketch? I tried to set some points in part design wb, but there are not reachable in sketcher tool.

[chrisb]

I don't understand your model, there are strange things in it: You have used "Pad" directly in a Part workbench operation. I thought you can do this only in a Body. Have you switched between 0.16 and 0.17?

To get the shape of the pins you are almost there: in Sketch001 you can use the half circles for external geometry references. You don't need ReferenceCut, ReferenceCut001,ReferenceCut002,ReferenceCut003. Besides you can put multiple things into one ShapeBinder.

[chrisb]

I have a simplified version here.
- Instead of cutting the singular pin I simply deleted it
- For the solid to be subtracted I used a ShapeBinder with two faces: one for the position of the plane and one for the circle which is used by means of "Pad up to face" for the length as well. So you don't have to guess the length of the pins to be removed
- The pins are in two bodies because they are two solids
- The length of both pins is controlled with Pad001.Length

[NormandC]

You're using v0.17 wrong.

Your Body contains nothing but shapebinders. The Pad is outside the Body, and you created two Part Cuts between the Pad and two of the imported solids.

To use PartDesign with an imported solid, you need to create a base feature from the solid. See PartDesign Body

[NormandC]

I don't understand your model, there are strange things in it: You have used "Pad" directly in a Part workbench operation. I thought you can do this only in a Body. Have you switched between 0.16 and 0.17?

I think that creating the Part Cut between the Pad and the imported solid is what ousted the Pad from the Body.

Brace yourself Chris, we are going to see a lot of those errors very soon!

[NormandC]

Here's how I think the model should be done in PartDesign. Unfortunately the color change to grey is unavoidable. It's an issue that will need to be addressed in v0.18.

If you absolutely need to keep the yellow color, then do not use PartDesign, and follow GeneFC's method.

1. First of all, select the 4 imported solids and apply a Part Union to get a single solid. BTW the main body is considered invalid by the Check geometry tool; but since you're only cutting the pins, it does not affect the model.
2. Create a Part container and move the Fusion object inside it.
3. Select Fusion and create a new Body. This effectively creates a BaseFeature inside the Body, linked to Fusion.
4. Create a sketch in the Body's XY_Plane. Draw a rectangle.
5. Create a Pocket feature.

I don't see the point in using separate bodies for the pins. This is supposed to be a single part, right? If you have pins separate from the main body, the STEP will be saved as an assembly of parts rather than a single part; maybe it will create problems in Altium...