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  • #16
    I agree designing and printing something is great.

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    • #17
      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:

      Click image for larger version  Name:	test1-FCAD.png Views:	2 Size:	8.1 KB ID:	4361

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

      Click image for larger version  Name:	test1-F360sketch.png Views:	3 Size:	52.0 KB ID:	4364
      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:

      Click image for larger version  Name:	test1-FCADsketch1.png Views:	3 Size:	4.4 KB ID:	4362

      Then a 2nd one like this:

      Click image for larger version  Name:	test1-FCADsketch2.png Views:	3 Size:	935 Bytes ID:	4363

      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.
      Ender5r
      Senior Member
      Last edited by Ender5r; 10-05-2020, 01:26 PM.

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      • #18
        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.

        https://www.geit.de/tmp/FrameExample.FCStd

        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.

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        • #19
          Thanks very much
          Geit
          Senior Member
          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?

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          • #20
            Originally posted by Ender5r View Post
            Thanks very much
            Geit
            Senior Member
            Geit. You've been a great help.

            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.

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            • #21
              I don't really understand that alternate method; at least not yet. However, one thing I noted in repeating the procedure a few times is how tricky the procedure can be. There are quite a few steps, and they have to be executed pretty much perfectly. I can do them from memory right now, but I wouldn't want to try to repeat them after having not done them for a couple of months.

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              • #22
                With that test shape I outlined earlier, I've been playing with filleting. It seems that, when possible, it's most advantageous to fillet sketches rather than paddings. 2 questions:
                1. is it true that filleting sketches is the best way?
                2. how do I specify a radius for a sketch fillet, other than dimensioning the distance between the locus and 1 endpoing?
                Ender5r
                Senior Member
                Last edited by Ender5r; 10-06-2020, 04:37 PM.

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                • #23
                  Originally posted by Ender5r View Post
                  With that test shape I outlined earlier, I've been playing with filleting. It seems that, when possible, it's most advantageous to fillet sketches rather than paddings. 2 questions:
                  1. is it true that filleting sketches is the best way?
                  2. how do I specify a radius for a sketch fillet?
                  Yes, it is the best way. Current FreeCAD has some issues with consistency, when earlier sketches get edited. E.g. when you take the first sketch and add a simple hole, it is possible that your model falls appart because of this issue (known as topology naming). The problem is that creating a circle in the first sketch will create new faces and new edges and cause FreeCAD to reassign previous set references on faces and edges wrongly. This is where fillets and chamfer fail first and tend to hop to a wrong edge, where they cannot work and the whole model stops being rendered properly. Same goes for sketches on faces of the model and external geometry.

                  This is the main reason I usually avoid external geometry as well as sketches on faces and thats the main reason I usually use datum planes as I can bind several sketches onto the same datum plane and if the datum plane goes haywire for some reason, I just need to reposition those and everything else falls back in place correctly. With a proper name of the datum plane it is easy to find the original position in case it fell appart.

                  But even with datum planes I tend to model around the origin, placing my DPs using known offsets like BaseSketch.constrain.FrameWidth/2 to get on the right side of a model.

                  This issue got a little better with recent FreeCAD releases, but it is far from being fixed. In fact this is the only issue that holds FreeCAD back right now. You can edit a model parametric right now using references mentioned above and it will work, but only until you edit something upstream of your build path. Then it silently fails.

                  There is actually an example in FreeCAD I use to check if the issue is still there. If you are on the start page of FreeCAD there are your latest projects and some examples. Load the PartDesignExample file. It looks like a key shaped castle wall. Now open the first pad named "pad" and enter the sketch within. You see a rectangle with an arc. Now make a small circle onto the radius of the arcs center. This should make a hole bottom to top in the "castles tower" and nothing else. If you close the model you will notice that the model looks different as the rectangular pocket moved from the top to the bottom of the model, due to the topology naming issue. The additional hole created a new face and the pocket got shifted to some random other face, which is on the floor of the model.

                  And now 2) Sketch filets are just normal segments of a circle. The tool just inserts them for you and sets a tangential constrain. Just click on the circular segment and define a radius. Done.

                  Here is the other way to create the frame without a datum plane, but with two pads:
                  https://www.geit.de/tmp/FrameExample2.FCStd
                  Geit
                  Senior Member
                  Last edited by Geit; 10-06-2020, 05:11 PM.

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                  • Ender5r
                    Ender5r
                    Senior Member
                    Ender5r commented
                    Editing a comment
                    Just tried release 23323. The topology naming issue is back.

                  • Ender5r
                    Ender5r
                    Senior Member
                    Ender5r commented
                    Editing a comment
                    And still present in 23463

                  • Ender5r
                    Ender5r
                    Senior Member
                    Ender5r commented
                    Editing a comment
                    Just tried the "castle key trick" with RealThunder's FreeCAD-asm3-Daily-Win64-Py3-Qt5-20210717 version. Drawing the circle in the cylinder on the right worked properly.

                • #24
                  I watched this video: https://www.youtube.com/watch?v=_GxJkB23ZHM. It helps F360 users adapt to FCAD. At one point he points out that 1 of the things being looked at for the next version of FCAD is support for multiple objects in 1 body. He also showed how it's possible to do joins and cuts by creating bodies, selecting them together, then using the join and cut tools. That is way more like F360.

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                  • #25
                    Originally posted by Ender5r View Post
                    I watched this video: https://www.youtube.com/watch?v=_GxJkB23ZHM. It helps F360 users adapt to FCAD. At one point he points out that 1 of the things being looked at for the next version of FCAD is support for multiple objects in 1 body. He also showed how it's possible to do joins and cuts by creating bodies, selecting them together, then using the join and cut tools. That is way more like F360.
                    I never used Fusion360 in my life! The only other CAD software I "launched" was Blender on MorphOS, just to see if it works.

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                    • #26
                      Soooooo, just now I decided to revisit the headrest purse/bag hanger, but this time using F360. I've avoided doing that up until now because I was determined to do it in FCAD.

                      Wow, what a difference! True, I do not have much experience with FCAD, but I don't have that much more with F360. Creating the hook in F360 was 100 times easier than in FCAD. It took me less than 10 minutes, and it was done using a single sketch. And, it also incorporates the "finger hole" I talked about earlier. Plus, it incorporates all the fillets I wanted, and they were absurdly easy to do.

                      Image captured from F360: Click image for larger version

Name:	HeadresrHanger1 v1.png
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                      Image captured from FCAD after importing a STEP file exported from F360: Click image for larger version

Name:	HeadresrHanger1_FCAD.png
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                      This experience makes it a lot harder to move away from F360. It also points out how FCAD needs a tremendous amount of development before it can compete with F360. Based on what I just did, and with the caveat that the list is not complete or even exhaustive, I take away these things that FCAD needs to incorporate or improve:
                      • when drawing a closed shape such as a rectangle or circle, adding dimensions should be part of the actual drawing process itself, not a separate function that has to be done later;
                      • the interior of all closed shapes should automatically become selectable faces;
                      • sketches must be able to have multiple closed shapes and not require the creation of separate bodies;
                      • closed shapes on a sketch need to be able to be extruded to different heights;
                      • filleting needs to be seriously improved.

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                      • #27
                        Originally posted by Ender5r View Post
                        [*]closed shapes on a sketch need to be able to be extruded to different heights;
                        In some points you are right, in others not. Like the one I picked. That is not the way it is intended to work.

                        What you do is checking how the windows desktop works and then blaming MacOS to do it differently.

                        This is a very nice channel, where more or less all CAD tools are shown.

                        https://www.youtube.com/channel/UC-C...NwC-3RBKUoAOQQ

                        I was amazed when I saw him model an WW Airplane or a Car in a few minutes using FreeCAD.

                        When it comes to testing builds, Fusion360 already fails as the simulation stuff is lacking in the free version. The videos in that channel show extensively what is possible in all CAD applications and he constantly compares the current workflow with the one used in other CAD tools.

                        The point is that you are used to Fusion and when I would swap to Fusion I would have difficulties to adapt my workflow, too.

                        On top of all that, keep in mind that FreeCAD is not developed by a company with hundreds of developers working 8 hours a day on the applications. FreeCAD gets developed by three hobbyists in their spare time plus a couple of people helping out and adding more workbenches to the mix.
                        Geit
                        Senior Member
                        Last edited by Geit; 10-07-2020, 07:08 PM.

                        Comment


                        • #28
                          Actually, I'm not picking on F360 or FCAD; they are just the current examples. When I say FCAD needs to be able to have multiple objects on 1 sketch, what I really mean is that any good CAD package should have this ability. The same applies to all the other points I made. It was just that I zoomed in on these ones because I noted how the 2 CAD programs are different.

                          I'm really not comparing apples (hehe) and oranges. I honestly don't care whether FCAD is designed to work with multiple objects on 1 sketch. My point is that it is the way it should work. That, of course, is just my opinion, but there it is. Oh, and my understanding is the next version will allow multiple objects per sketch. Whether it will allow different padding heights, I don't know.

                          I'm really not used to F360. I only have a few hours more experience with it over what I have with FCAD. It was very hard to get even a bit of a feel for F360, but FCAD has been much harder.

                          Sorry, but I don't make allowances because FCAD is developed by 3 hobbyists. However it's developed, the bottom line is my experience using it. I'm looking at the whole CAD thing from an agnostic point of view: which one is better to use, regardless of cost or how it's developed. No, I would not pay $300+ per year to licence F360, but I would pay $50, which is what I do for my Untangle UTM. I do admire & applaud the FCAD developers for their efforts. It is a wonderful thing they're doing, but their product is not where I believe it should be. I give them kudos, but I won't make allowances. I don't believe the idea of Open Source is to create sub-standard products. In the projects I worked on, my standard was to be state-of-the-art, not so-so-OK.

                          Thank you for the link. I will definitely look at it.
                          Ender5r
                          Senior Member
                          Last edited by Ender5r; 10-08-2020, 06:43 PM.

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                          • #29
                            Geit
                            Senior Member
                            Geit, I just wanted to update on the Joko Engineeringhelp videos. There is no doubt the guy is a maestro, with both FCAD and Solidworks. I doubt I could ever achieve anything close to his level of skill & expertise. I did note that he pointed out how FCAD is weaker than Solidworks when it comes to filleting. So, for the purse hanger, I guess F360 was my best option. That said, I'm not giving up on FCAD, at least not without giving it a good deal more effort.

                            I'm going to watch more of Joko's videos to see what I can learn. I'm particularly interested in how he uses the XY, XZ, YZ, and Datum planes to orient different sketches in a project. I'm pretty sure I've been over-complicating my FCAD bodies with sketches.

                            Again, thanks for pointing me to his videos.

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                            • #30
                              Yeah, at first I used references to faces, which - as I mentioned above - cause trouble and had a very bad time. Then I used DatumPlanes as work around, but they became very handy.

                              I now use them all the time, even sometimes when modeling on a standard plane to give it a name. Linking multiple sketches to a side of a model is just saving so much time on the long end.

                              Did this today:

                              Click image for larger version

Name:	TronXYFanMount.jpg
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                              It is a two part fan shroud for the default TronXY X5, which is just blowing sideways onto the hotend, which currently needs kapton tape to be insulated from the air stream. This should be far better, cool both sides of the model and not the heater block.

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