Extend a face, bringing along supporting fillets

[xbit]

I want to extend a face from a model, and have the supporting fillets extend as well, in order to support this operation.
Now, what do i mean by that....

1.png (19.82 KiB) Viewed 988 times

Suppose i have this model and i want to extend the highlighted face to the left.
Extending the face is something i did with python or GUI tools but it doesn't look right.

This picture shows only the face extended:

2.png (22.11 KiB) Viewed 987 times

There is a problem though. All the supporting filets have stayed behind. If we tried to extend the fillets as well we get this:

3.png (27.74 KiB) Viewed 987 times

Is there a way to extend our original face, but move the fillets as well to support it? It's like the whole side of the model will be pulled.

This operation looks like scaling but it's not.

Let's see what will happen if we try to scale:

4.png (22.55 KiB) Viewed 987 times

As you can see, the supporting filets moved along, but they got scaled (obviously). If you look at the selected fillet, it is double the length that was previously.


What i want is to pull the side of the model, moving the fillets along, in order to support is, but don't change their length.
In other words, the geometry will stay the same, but the object will have been elongated from one side...

I hope i said it clear, it isn't easy to express visual context throught text....

Is there such an operation in FreeCAD?

[xbit]

I do not know why images are not visible. I uploaded images to imgur and pasted the link inside the space between the tags...

[drmacro]

use the add file tab below the post editing window

[openBrain]

I do not know why images are not visible. I uploaded images to imgur and pasted the link inside the space between the tags...

Because an imgur URL isn't an image, it's a link to a webpage that (among other things) displays an image. Using the forum attachment feature is definitely the way to go.

[chrisb]

I would cut the object vertically in the middle, e.g. with a face and slice apart, move he pieces and fill the gap which is now easier because the cut is not angled.

[xbit]

Thanks chris!
I got the idea visually in my mind.
Is it easy to list the tools that would provide that functionality?

Which is the tool for doing the face and slice apart etc?
I am super new to FreeCAD

[openBrain]

Thanks chris!
I got the idea visually in my mind.
Is it easy to list the tools that would provide that functionality?

Which is the tool for doing the face and slice apart etc?
I am super new to FreeCAD

* Add a Part/Plane in the middle
* Part/SliceApart your solid with the plane
* Move one of the obtained fragments
* Make a Draft/FaceBinder of the inner face that has been exposed by the slice
* Part/Extrude the FaceBinder to join both fragments of the original object

[chrisb]

- Switch to Sketcher workbench
- Make a vertical line in Sketcher where you want to cut.
- Switch to Part workbench
- Extrude; this will give you the face for the slice
- SliceApart will give you the two parts
- Switch to Draft workbench
- Create a FaceBinder on one of the cutting faces
- Switch to Part workbench
- Extrude the FaceBinder

[jmaustpc]

With the normal FreeCAD work flow, you would extend the face of the solid on which the fillet had been applied, so you would go back in your history and just edit that, it some case you would need to repair or replace the fillet after the solid has been extended, since the edges of the extended solid may have a different new internal numbering that they had originally thus causing the fillet to be applied to a wrong edge, however if you are just increasing the length you could be lucky and have it just work, also if you have the same fillet on all edges then it also would likely just work.

The workflow that the others are suggesting is assuming that you have a non-parametric solid, perhaps for example a solid imported from a STEP file or similar.

In this example all you have to do is change the value contained in the spreadsheet Cell A2 with an alias of "length_of_object", and FreeCAD will extend it in the manner you have asked. The Draft WB clone will always be two times the length of the first object, in the Y axis direct.

strechPDobjectexample.FCStd

(285.17 KiB) Downloaded 13 times

Also note that a Draft WB clone can be independently scaled in the direction of each axis, this will also work to lengthen your object and will include the fillets. I think the developer once said that if you scale a Draft Clone in different amounts per axis, then lines get converted to splines (straight still splines), if that is so, then it may or may not cause any further complications. If you want to know how that works in Python then have a look at the Draft Clone code as it is written in Python.

OS: Ubuntu 18.04.5 LTS (KDE/plasma)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.
Build type: Release
Branch: unknown
Hash: f7532b91d47f1048f54a42038ac5595592ff76a4
Python version: 3.6.9
Qt version: 5.9.5
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/Australia (en_AU)

[xbit]

Hello jmaustpc .
I saw your post and there are several things that are not clear to me.
First of all, how do you generate that spreadsheet, where i can modify the axis?

Then spreadsheet variable changes the axis of the original object, and then the clone changes that amount X2, am i correct?

But if you see at the second object, the size of the surrounding filet has changed as well, compared to the original (it is doubled).
I want to extend the face, and the suuporting fillets should stay the same width, if you look at my pictures attached you will understand.

But when i change the length of the original object (via your spreadsheet). Then the original object just extends the face, bringing along the supporting fillets together, WITHOUT changing their width. This is exactly what i want to do.
So, is this achievable? How exactly did you generate the excel spreadhsheet?