Anyone Up For A FreeCAD Challenge

And now for something completely different. People have, as we all expect, come to the forums for help and guidance around everything to do with 3D printing. But, I don’t think there has actually been a challenge issued. So let me be the first.

In response to all the people who love FreeCAD and would like to see me use it (at least I think that’s why they tout it’s benefits), I spent last night and most of today trying to create a hanger for hanging purses and shopping bags from the back of car seats. It uses a headrest post to hold the hanger. I have attached the FreeCAD file for those who want to have a look (I had to upload it as a Zip because the forum software won’t let me upload FCStd files).

Here’s the challenge. If you look at the hanger in FreeCAD you will see that most edges are filleted. The ones that are not filleted are the problem. If I try to fillet them, FreeCAD generates errors in the Report View and then crashes, totally quitting. I tried v0.18 & v0.19. In particular, the line where the round sleeve meets the flat base cannot be filleted, like it is at the other end of the hanger.

One reason I chose this project to try in FreeCAD is because, in order to protect purses and such, I really think it needs to have the edges filleted and, truly, openSCAD just doesn’t do filleting well at all (I was warned, and those issueing the warnings are correct).

A 2nd reason is that virtually every car seat hanger I could find on Amazon and other sites has an opening to allow it to be fitted around the headrest post. My wife has had several of these, and they always end up coming off, which leads to the inside of the car being polluted with the residue of the blue language that comes out of her mouth. [SIZE=20px]?? [/SIZE]Thus, my design is solid around. It does require popping the headrest off the seat, but that’s a minor inconvenience, since it only needs to be done once.

A 3rd reason for choosing this project is that I believe it’s something virtually every forum member could use in their own life.

Once the filleting issue is resolved (which I’m sure all you 3D geniuses will do), I plan to fully parameterize it.

I’m also thinking of putting a notch in the clip end of the hanger, so that it will be easier to get a finger in to grab the purse or bag straps.

So, what do you think. Anyone up for the challenge?[SIZE=28px]?[/SIZE] (288 KB)

Challenge Accepted! :smiley:

First of all. Do not use the hole tool, when a simple circle in a pad sketch can do the same. I never used the hole to in any of my projects.

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I remade your design in just three pad operations (extrusions) and two fillets with all the requirements you wanted.

The base pad, the ledge pad and the hole pad. To achieve the fillet I did a little trick. I added the fillet to the base plate, so it is there before the circular padding gets added. Since a simple padding would now create a grove, I lowered the base for the pad operations by fillet-diameter/2. That way the padding just extrudes through the fillet where required and there is no seem from the surrounding fillet visible anymore.

The model is parametric, but I did cheat a little as some fillets are only 50% of the values defined in sketch. However. You can change the measurements in combo view, where they appear as plain name.

The file can be found here:

The Process took me about 30 minutes. Mostly because I had to swap forth an back to get your measurements right. The design itself is a little dirty as I used helper lines within sketches as reference storage. Normally you would create a spreadsheet with all the data and reference that. However, I find it helpful in such small designs to have most measurements in just one sketch and only define the pad/extrusion/pocket height within the sketch used for the operation, like I did in hole and ledge sketches. Also Spreadsheet are a little user unfriendly in 0.18. 0.19 is far better in this department, but still a little confusion. :smiley:

What is my price? :smiley: Did I win a car?

Glad someone accepted. I’m really hoping it will help others get a handle on how to use FCAD. I’ve had a very quick look at your file, and it’s very interesting indeed. I think I will learn a ton from it, although I’m sure I will have questions. I toggled all the pads & the sketches so I could see all the sketches together without anything else. The first thing I noticed is how the sketches are on different planes in space. I wasn’t aware you could do that, and I still don’t know how it’s done, but I’m sure I can find out, now that I know what I’m looking for.

The bigger question is why use sketches on different planes? I think I’m going to go to my desktop 'puter in the basement, the one with two 30" screens and fire up 2 instances of FCAD, so I can try to duplicate what you did.

Seriously, many thanks for joining in. As I said, I feel I will learn an awful lot, especially about how to approach projects.

Well, you can move sketches itself, but I prefer creating a datum plane, as it gives structure. You can also angle and orient them in 3d space as you wish.

In this case I needed to start on the level of the fillets to “overwrite” them. I could have started from the bottom up, but then I would have needed an additional fillet just for the bottom plane. This way I create a base and put fillets all around it before continuing the process.

Ha. Now I have to find out about datum planes: like, what they are, and how to use them… more homework :slight_smile:

They work exactly like your XY, XZ or YZ planes. The only difference is that you can place them where you want and in which orientation you want them.

Thanks for all of the lively discussion. This is on my to-do list. I was going to dive into F360 until they decided to cut off home users. I just need to get some other projects finished so I can start.

Welcome to the challenge @woodwaker_dave. I’m kinda hoping Irv will take up the challenge too (without looking at @Geit’s solution :slight_smile: ). I suspect there are a thousand ways to skin this cat. It would be interesting to see the different approaches; one of the main reasons I decided to post the challenge.

@Geit, On the BaseObjectPadSketch, did you use Fillet to round the 2 corners at the end opposite the hole, or did you use 2 circles and make the ends of the lines tangent (it kinda looks like tangents)?

I used the sketch filet option in sketcher. I basically drew the top circles and drew three straight lines. Then I used the filet tool and clicked onto the corners at the bottom. I could have used circles as well, or the multi line tool. All three methods result in the same sketch.

Ah. Well, there you go. I didn’t even know there is such a thing. I hoped there was, but hadn’t found it to date. That should get easier now that I’ve added the Accessories menu item with Toolbar style. I used it to add text under the toolbar icons. Voila, I found the Sketcher Fillet icon.

Usually they are easier to use, but since your shape was triangle I had to add a helper line to maintain an accurate size, when the lower fillets are set.

When using the multi line tool you can press “m” and toggle through several possible line options. That is a thing I did not know until recently.

I just downloaded freeCad but I am not too hopeful about learning to use it. I don’t even have a car so I probably wouldn’t waste plastic printing this out. I can’t even figure out how it works.

Well, you could print some for relatives & friends. That’s one of the reasons I uploaded the file, so that, once the design is finalized, everyone can use it for themselves, or for others. Also, I want it to be fully parametric, so others can customize the design to fit their situation.

CAD is for sure not easy to start with. FreeCAD isn´t for sure. But you can perform leaning by doing and there are nice tutorials on YT showing basic sketching and using. Even @DrVax did a videos on the topic. Its kind of like tinkercad, where you sketch something and pull it into the third dimension.

It is just nice to hold something unique in your hand that you designed yourself to fix a problem, which nobody else could or would fix for you.

I agree designing and printing something is great.

So, I’ve been working intensely with FreeCAD for a couple of days now. I must say, I’m finding it extremely frustrating to use. I assume this is because I don’t know what I’m doing. So, I want to post a test object I created in both F360 & FCAD, describe what I did, and see if anyone can point me to a MUCH better way to do it in FCAD.

First, here’s an image of the finished object:

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Now, here’s a sketch of the object done in F360:

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To extrude/pad this object, all I had to do was click the face (interior) of the smaller section and click on Extrude (all closed shapes in F360 automatically create selectable faces). I entered 5mm in the popup box and that part was done. Then, I clicked the face of the larger section and again clicked Extrude. I entered 10mm, clicked OK, and again, done. I did NOT have to constrain the object at all. I did NOT have to create a 2nd sketch (it was all done using the one sketch). I did NOT have to activate External Geometry.

Now, on to FCAD. In order to get the object, I had to create 2 separate sketches, the first one like this:

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Then a 2nd one like this:

[ATTACH=JSON]{“alt”:“Click image for larger version Name: test1-FCADsketch2.png Views: 3 Size: 935 Bytes ID: 4363”,“data-align”:“none”,“data-attachmentid”:“4363”,“data-size”:“medium”}[/ATTACH]

However, in order to get the 2nd sketch to be perfectly aligned with the 1st sketch, I had to use the External Geometry feature, to make the points at the 4 ends of the diagonal lines selectable.

Then, in order to be able to extrude/pad the sketches, I had to add a bunch of dimensions in order to full constrain the sketches. If FCAD can extrude non-constrained sketches, I’m afraid I don’t know how. All I get if I try is a blank viewing window. Oh, and before anyone tries, please don’t tell me that having to fully constrain before extruding/padding is a good thing… just don’t.

If I try to extrude/pad it all done in one sketch, I get an error about not being able to pad a broken face. After face-palming myself so many times, I think I may have broken my own face.

The bottom line is creating this object in Fusion 360 was really easy and quick. Creating it in FreeCAD was much harder and took at least 5 times longer. Please, someone tell me I’m going about this all wrong, making it 10 times harder than I need to.

UPDATE: OK, I was just able to Pad in FCAD without constraining. Whew. I’m still exploring it, but I wanted to update immediately, so no one has to waste their time explaining it to me.

UPDATE 2: I’ve figured 1 way to pad the 2 segments separately, by creating 1 sketch in a Body, then creating a 2nd sketch right under the 1st one, in the same Body. I still have to use External Geometry to select the 2 diagonal lines, then fill in the other lines. Then, I could select each sketch, in turn, and pad them out to different dimensions. Still not as easy as F360, but better than before.

You can basically do what you did with fusion and place the design in one sketch in FreeCAD. The only difference is that you need do “disable” the small diagonal lines before performing the first extrude. You do that by turning them into helper lines. Then you can extrude the entire frame to full height.

Next step is a second sketch, where you get the two small lines you previously turned into blue helper lines and draw the four lines. The sketch will be fully constrained, as the dimensions and orientations are in the previous sketch. Then you perform a pocket on the second sketch to remove material.

In FreeCAD you cannot simply extrude multiple parts of one shape in a different way. You can only extrude or pocket all white lines.

I used a datum plane so create a visible plane. You could have extruded the pocket from the bottom up, too. I also did not use proper references for the height of the model, so the datum plane will not move when changing the height of the base frame. This is just a quick drawing without any proper measurements.

Thanks very much @Geit. You’ve been a great help.

I tried to replicate your drawing. I drew a rectangle, then another one inside the 1st. Then, I drew the diagonals and converted them to Construction Lines. Then I used Pad to extrude to 10mm. Next, I created a Datum Plane on the top face. Then I created a sketch on the Datum Plane. Using External Geometry, I clicked on the 2 bottom lines to make them accessible. I used Polyline to outline the bottom 2 lines and the diagonals, toggled the Datum Plane invisible, then editted the sketch. I made sure the 2 points at each of the 4 corners were coincident. I closed the sketch and used Pocket to cut the front wall down to 5mm. Afterward, I figured I didn’t really need the 2 Construction Lines.

Is that the right procedure?

Yeah, that is the way I go. There are - as always - other ways in CAD. The construction lines are not really required. I left them in, just in case you want to add measurements or angles tied to them or to get a more real world top view, when designing. As I mentioned previously I like to have a more or less complete sketch with all dimensions, which I can reference by name from everywhere. I also would have added a vertical or horizontal blue helper line named “FrameHeight” to reference from the pad and pocket tool to import the measurement.

You can also turn more lines into construction lines and extrude a full height “U”-Shape of the frame and then, without using a datum plane, just pad the closing element in half height. That way no datum plane and no pocket is required to get a clean x/y oriented object.