DRAFT goes wrong / any way to automatically smooth out lines to curves/arcs ?

[ovisopa]

I'm trying to make a 30 degree angled "wall", I modeled just one other drawing and it worked ok using the DRAFT option, but in this case the draft is not doing what I want in the corners of the drawing, the other sides are ok, but the corners are not.

Also is there a way to automatically transform straight lines with many segments, or curves with many segments and convert them to one/multiple curves or arcs ? The drawing is an imported DXF, in other software I use, I have an option called ARC FIT and it does reduce the number of points a lot, is there any similar option in Fusion ?

[HughesTooling]

I wonder if the is a really small surface in the corners you haven't selected. Any chance you can export your f3d file and attach to this thread? Fusion doesn't have any arc fitting feature, you will get a better surface if you trace over your sketch with a spline. Using splines you'll end up with only 3 surfaces for the outside shape and it'll be a lot nicer to work with.

Mark

[ovisopa]

In this case it seems it worked better with the CHAMFER function, I offset the contour by 2.3mm and than I aplyed a chamfer with 2 dimensions, I also tried Chamfer with Distance and angle option but I got an error, but using "Two distances" instead,  it worked.

In all those models I make I need to have a specific angle for the wall, and I know the wall height, if there is another method to do it, let me know. With draft it was easier as I only inserted the angle and that was it, with chamfer I need to offset at a correct distance and than apply a chamfer.

 So I have to manually do the trace ? This is not a good news 🙂

[HughesTooling]

If you zoom in to the corners on your sketch you'll find this. If you delete the short line it'll fix the problem.

Mark

[ovisopa]

Ohhh .. so it's again "a problem" in the geometry client sent me. 

In fusion is there any "clean" drawing function ? Something that can remove / point's that are to close one to another ? In this case the distance between the points is 0.001 mm, it will be great to have a function to clean the drawing to a value I can enter, like 0.1mm.

I did zoom before posting, but I haven't zoom enough 🙂

I think while I was watching the tutorials, or lessons I seen a smoothing option, but it was applied in the CAM section, it did exactly what I wanted, it reduced the number of segments, so that might be available only for the CAM section, and not the model section.

Thank you.

[ovisopa]

I tried to move the point over the other one, and it didn't do anything, also tried to remove the small segment between the points and than move the end pointover the other but I couldn't do it either.

The only way to move it was by dragging, but I don;t have any precision and it doesn't snap exactly over the other point. Is there a fix for this ? Other than switching back to Cambam, clean the drawing, and than export it and start over with the cleaned drawing

[HughesTooling]

Yes there is smoothing in the CAM machining ops but there are no tools in the model workspace. If you look at your example above where you used arc fitting you can see there is a symmetry error. You will always get far better results tracing with spline and using a mirrored copy of the spline for the other side. See screencast below showing how I'd go about creating the solid block from your sketch. By the way don't make copies in you sketch if you can help it, you will get better performance copying the solid bodies\faces. I've attached the file from the screencast, you might want to put in a bit more time making sure you're happy with the traced profile. With practice you'll find tracing quite fast.

Mark

[HughesTooling]

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@ovisopa wrote:

I tried to move the point over the other one, and it didn't do anything, also tried to remove the small segment between the points and than move the end pointover the other but I couldn't do it either.

The only way to move it was by dragging, but I don;t have any precision and it doesn't snap exactly over the other point. Is there a fix for this ? Other than switching back to Cambam, clean the drawing, and than export it and start over with the cleaned drawing

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Try using extent to extend the vertical line ten use trim to remove the unneeded lines.

Mark

[ovisopa]

Thank a lot Mark .. at minute 1:36 in your screen cast  I was: whaaat ... wow 🙂 

So you would suggest to redraw the objects that generate errors in the 3D model

[HughesTooling]

I would just recommend redrawing anything that is made from lots of line segments like you had. The single spline I ended up with for each side will be a lot easier to work with, things like adding draft angles and fillets will be a lot more reliable. 

Mark

[ovisopa]

Mark, I followed your screencast and made myself a new drawing using the same principles (copy the initial drawing using spline and mirror, extrude one part, use a rectangular pattern to copy the extruded model) and it came out nice, but now I wanted to make a small interior offset of just 0.2mm and I can't select the 2 splines and the connecting line all at once, I could select the initial sppline and the connecting line, but not the mirrored spline, if I make the offset each spline/line at a time there are some extensions at the end of the line/splines. 

If then I trimmed that extensions, I got an warnign that one constrain was removed because of the triming. Is the way I did not ok, is there another way to make that internal offset ?

 Also when I tried to extrude that offset, I noticed the extrude was not applied to the other patterned solids, is there a trick to apply the modifications to all solids? Or I have to first finish all modifications to the initial solid and only after that to make a pattern ?

[HughesTooling]

Not sure why the offset didn't work for you, I just tried with the file I attached above and had no problems. Can you upload the f3d file you're working with. 

You need to roll the timeline back before the pattern if you want all copies to end up with the extrude cut. I've made a screencast below, I was surprised I didn't need to edit the pattern and select the new extrude cut. You might need to add the extrude cut to the pattern if it doesn't work for you.

Mark

[ovisopa]

Awesome ! In the mean time I have deleted the pattern and made it again after applying the interior extrude, but it was great to understand better where I could use the the advantage of the timeline  (as it happen multiple times to be pissed of because of the timeline, when I wanted to modify something, let's say draw a new line at the same distance or angle with another line that was added after the initial drawing, when I clicked edit sketch on the initial drawing, the new one dissapeared and it was more difficult to draw to that point, or at the same angle - but I'm sure it was me doing things the wrong way, anyway, I'm learning daily now 😄 ). I didn;t knew that if I scroll the timeline back, the modifications will apply to the elements created after that point. 

I attached my drawing, I'm curious what I did wrong 🙂

[HughesTooling]

I made one screencast to show there's an overlap where the splines should meet. You picked up a midpoint on the arc from the sketch you were tracing. There was still something odd with the symmetry and after a bit of experimenting I found your symmetry line didn't have a horizontal constraint, I show this in the second screencast. I think this was probably the main issue. 

Fixing the crossing splines.

Adding the horizontal constraint.

Mark

[ovisopa]

Thank you Mark for all your help with those screencast !! 

I have a new model to mill, and of course, as always, I have new issues/challenges 🙂 I tried to create the 3D model from the provided DXF but it failed when I tried to apply chamfer or draft to the exterior wall. I tried to simplify the drawing with CamBam, but even with less points I couldn't apply a draft on that side wall.

So my last option was to redraw again the part, I did and the extruded model looks good, but weird, now when I try to draft that wall, it works to an angle of 29.9 degrees, it does what I want , but if I want to use a 30 degree value it fails, and the wall remains straight, not angled. 

I think in this case I'll be ok, I will mill using the 60 degree end mill, the difference will be quite small, but I really want to know what could be the cause, because I also don;t know why it fails so close to what I need, if I needed that draft to a 40 degree angle, than I couldn't move over to the next step: CAM

I'm attaching the model and a screenshot

[HughesTooling]

The problem's caused by having 2 points close together where there's an internal curve, if you delete the 2 fit points in red boxes it will work fine. At the moment you can see the offset at the bottom of the taper is coming to a point, any father and they'd overlap and cause a self intersection. You'll have this sort of problem adding fillets and chamfer as well, just something to look for if you can't go over a certain size.

After removing the fit points you will need to adjust the handles on the spline to fit the original sketch.

[ovisopa]

So frustrated again .. I did redraw the shapes twice, but still can't make the draft wall at 30 degree 😞

Anyone around to take a look ? I lost about one hour and 20 minutes trying to make this model, I give up now and start working on other files 😞

Thank you.

[TrippyLighting]

Of course that does not work. The small fillets at the end of the profile would collapse to a negative value when that geometry is drafted.

If you add sharp corners to the sketch as shown in the screenshot it can be drafted fine to -30 degrees (inwards).

Then you can decide what to do with these sharp ones. You can apply a constant fillet or if it suits the end product better a variable radius fillet.

[HughesTooling · Accepted solution]

@TrippyLighting the taper should go the other way and I think it's failing because @ovisopa is using arc fitting in another program. I the earlier posts in this thread there are other examples where the arc fitting is creating bad tangency and small segments that collapse with big draft angles. @ovisopa you will find it quicker to import the polyline and trace with splines and arcs like I demonstrated in the earlier posts. Also for parts with 4 way symmetry you should be able to just recreate on quarter and mirror.

Here's a screencast using what you have and mirroring but the left to right symmetry is not good.

[HughesTooling]

OK just noticed I can add draft while extruding but can't add a draft to the extrusion if it's parallel. If you have chain select enabled when you pick the side faces you can see the bad tangency.

Screencast show bad tangency with original sketch and good tangency after tracing in Fusion.