How to get a 'taper inward angle' draft clearance

[Rod]

I use Fc V0.16, without Body , Datum etc... I use your sketch itself

Yes, I started with v16 doing what you are doing...now trying to use v17 Body and incorporate v16 knowledge as well. You should give v17 a go.

[Rod]

Going to correct myself for trying to do as many steps in Part Design WB/Body as possible.

My understanding, the reason for using Part Design WB Body is that this is the path to the Assembly workbench(?) So would work done purely in Part WB be usable in the Assembly WB?

As GeneFC indicated earlier, use the Placement in Comb View to manipulate sketches made originally outside the Body. Starting the sketch on a Datum Plane will not allow you to use the Placement in Combo.

Tree using Placement instead of Datum Plane.JPG (31.63 KiB) Viewed 1164 times

[Rod]

First off, got to ask meme2704 what is the yellow head on your signature?

For the sake of completeness I've attached some pictures as I followed ppemawm's Draft method. Works well - thanks ppemawm. The small arc corner also showed problems in ppemawm's example if you look close, so I converted the arc corner to a square corner for the Draft exercise, then filleted it later. i also played with Thickness, but did not include pictures - you've suffered enough

What have I got out of this whole thread? Concern about workflow design.

I'm not sure, but is there a valid view that sometimes you will definitely need to do some things outside the Part Design WB Body disciplined approach? If so what are they? And will they wreck your work already done in Body if you have to include these exceptions at a later date? If you are doing serious work with FreeCAD then you need to know so that work flow can be planned.

My first impression was that I had to step outside the Body method if I wanted to do taper angle, that is use Part WB Extrude. Then drag the Extrude into Body as a Base Feature. The very name 'Base Feature' implies it should be the first thing put into the Body, and not something half way through a job.

For arguments sake lets say you have already done several days work in Body, but find later, unexpectedly, you need some tapered addition via Extrude. You drag the Extrude into Body as Base Feature, to find that Base Feature cannot be blended in with your previous work. Your only choice is to delete all your previous work, then rebuild it onto the Base Feature.

Can Base Feature be converted to simply another sketch on Datum Plane inside Body? Is it something that should be asked for?

Thankfully some way through this thread ppemawm pointed to Draft and Thickness, designed for the new Part Design WB discipline, designed to replace the Draft WB Extrude, it would seem.

I'll dump the pics first then add comment.

01 Sketch in Part Design Body.JPG (36.34 KiB) Viewed 1147 times

02 Padded sketch.JPG (47.56 KiB) Viewed 1147 times

03 Select faces then Draft tool.JPG (28.43 KiB) Viewed 1147 times

[Rod]

It's a worry. Your model will disappear after selecting Draft. Select the Neutral Plane button to bring model back into view.

04 Select neutral plane to bring sketch back.JPG (50.53 KiB) Viewed 1146 times

05 neutral plane selected.JPG (56.99 KiB) Viewed 1146 times

Your sketch will disappear again. Select the Pull Direction button to bring your model back.

06 Pull direction selected.JPG (73.58 KiB) Viewed 1146 times

07 taper applied.JPG (56.89 KiB) Viewed 1146 times

Check that the model conforms to the dimensions you have set out in the sketch - unless you are intending to thicken walls as in ppemawms example.

08 check taper conforms to sketch dimensions.JPG (66.98 KiB) Viewed 1146 times

[Rod]

09 Fillet applied to problem corner.JPG (30.18 KiB) Viewed 1145 times

ppemawm's exercise is a little different. The sketch appears to sit between two walls. ppemawm added thickness to the wall when hollowing the gearbox - this thickness runs from the white line to the internal wall.

The outside wall also seems to sit some distance from the sketch - but this is really the result of direction of taper.

If you want the Draft to accurately match the dimensions of the sketch then you need to take care with direction of extrusion and direction of taper which both have 'reverse' options.

10 ppemawm's draft.JPG (19.38 KiB) Viewed 1145 times

[meme2704]

meme2704 what is the yellow head on your signature

It's jok from my grandson for my 70' , the text is "befor your are old, now you is very old"

[ppemawm]

For arguments sake lets say you have already done several days work in Body, but find later, unexpectedly, you need some tapered addition via Extrude. You drag the Extrude into Body as Base Feature, to find that Base Feature cannot be blended in with your previous work. Your only choice is to delete all your previous work, then rebuild it onto the Base Feature.

One thing you can do, awkward as though it is, after you create the body sketch and the Part>Extrude on the face you want, drag the Extrude that gets kicked out of the body into a new body then you can PartDesign>Boolean the two bodies. In that way you can carry on with further PartDesign features without losing any work.

Picture1.png (98.52 KiB) Viewed 1129 times

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.13826 (Git)
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Branch: master
Hash: 3b02ff2a9481f0883063c7e24c312978ef0ce642
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: English/UnitedStates (en_US)

[Rod]

you can PartDesign>Boolean the two bodies

Ahhh! Interesting way forward. Thanks for the tip. Oh, does that mean i should make some more screen shots...

It's jok from my grandson for my 70' , the text is "befor your are old, now you is very old"

My only just adult kids think anyone over 30 is old. I tell them if I had them when first married they would be heading for 40 in a few years - that screws their faces up!