Trouble with fillet around awkward shape

[Hend-Eng]

Hi,

Please see attached screenshot. 

Re-creating a 1920s front axle from drawings and for some reason F360 cannot produce a fillet around this bracket / cylinder intersection. 

I was previously able to do it before I added guide curves to give the rectagular bracket it's proper curvature, 200mm radius; with the previous 2D curved faces I could fillet sucessfully.

Are there any workarounds available?

Without the 3D curves of the rectangular bracket the finish machined item just wont look as it should.

Workflow was to make a 1/4 of the axle, sweep the half cylinder and loft the rectangular sections from 2 planes with guide rails in 2 planes to get the right shape then mirrored the section to create one half.

Rads required from R10 to R30.

[TheCADWhisperer]

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[TrippyLighting]

Can you share your model ?

[Hend-Eng]

Thanks for the swift response guys! really appreciate it.

File attached for your delectation and also a snapshot of the drawing to give you an idea of the design intent. I've tried all sorts, it's just a few of the segments it can't get along with.

R10 and R30, bit vague in some respects but these things were originally forged and filed into shape. If a solution could be found to blend along the length of the chord to get 10 at one end and 30 the other, smoothly, that would be great.

As I said, when the rectangular shape had 2D faces, it worked.

[Hend-Eng]

 With the "straight" 2D sides to the rectangular bracket, no problems.

@TheCADWhisperer @thecadwhispere

[beresfordromeo]

Hi @Hend-Eng 

I am no optometrist but I am not really sure that this is model best tackled using the fillet tool. It could be that it is possible to do with a variable radius fillet but the likelihood is that it will take you some time and a divorce before this works.

There are several ways that you could approach this and I am sure that others will have plenty to say on that but I thought I would demonstrate a sort of dirty approach. Ideally you would restart the model to properly dictate the parameters of the fillet you want but I think that in order to get you a solution without messing too much with your original sketches this will do for now. Besides the dirty approaches are useful when you inherit designs and need to make changes such as these.

I have included a screencast and some instructions below however please feel free to ask any questions or criticise.

1 At 0.11 in the screencast I have demonstared a sketch I created on Plane 2 and named YZ Cut; this is on order to cut and prepare the rectangular part Body 15  for better transition to the pipe part.

2. I also created another sketch (see 0.15) called XZ Cut on the XZ Plane for the purpose of cutting the pipe part Body 1.

3. At 0.47 I am showing how I changed the loft that you created for Body 15 to become a New Body rather than a Join. These will keep the two bodies separate so that we can create the transition between them to reflect your design intent, a smooth transition with a variable fillet.

4. At 0.58 I am demonstrating how Body 15  was cut using the spline in YZ Cut , creating a new body (Body 16)

5. Same again at 1.13 but this time cutting the pipe part (Body 1 ) resulting in a new body (Body 21). 

6. At 1.29 I am attempting to demonstrate one of the important details of this method, in order for the loft work I have found it is good practice not to always use a single spline as normal but to use a number of splines to match the feature that you are attempting to loft to. This means that when the cut is made of the Body 1 , the resultant body Body 21 will have the number of edges that is required to make the lofting work. Lofting between surfaces with very different geometry works better when the number of edges is equal even if one of the surfaces you are lofting from is a single continuous curve. At 1.37 through to 1.39 I am showing how I achieved this with four splines each tangent to the next rather than using a single spline. I think that this is an important and often overlooked aspect of surface modelling.

7. The upright lines I am showing at 1.50 are to demonstrate how this geometry can be used as a way of viewing and contolling the spline points further down the model so that you can tweak the cuts to make your transition as you would want it to be.

8. At 2.09 I am attempting to show the first loft in the process using lofting in the surface environment. Had I approached this model in a different way this could have been a loft in the Solid environment but this is just a way as I said earlier, there are others and undoubtedly better ways.

9. If you look at 2.18 you can see that I can only use a tangent profile for Profile 1, the geometry not able to produce an G2 curve because it is too tight in that section, with some extra work however this would be possible. I am pointing this out because this is a common cause of failure for lofts.  Sometimes you can get arround this by adjusting the tangency handles but perhaps it is better not to get into this for this problem. I will try to demonstrate this one day if I get the chance.

10. The second loft at 2.50 has less strenuous transitions so is able to be G2 between both profiles.

11. At 3.06 I have demonstrated the command to stich these two lofts together to create a surface body, Body 24. Note the tolerance slider is fairly loose here. Sometimes to get a result it is better to perform more than one loft and stich them together rather than persisting with a single loft that keeps failing. 

12. .At 3.27 is a straightforward demonstration of the Create > Patch of the back of the body. I don't think I need to detail this except for mentioning that it is a good idea to turn off chaining of your patches are failing and also paying attention in case the edges that you are trying to create include virtually invisible edge that are not obvious but will make any suface loft or patch fail if they are not included in the chain. I am sure this has been the cause of frustration for many beginners.

13. At 4.00 I have shown the use of the combine tool to create a single solid body. This is a useful tool, easy to overlook and I thought worth a mention.

14. The rest of the screencast is a Solid > Create Mirror to create Body 27 from Body 16,  a Create Extrude.and a Create >Fillet. Nothing comlicated there.

i5 To my shame I was unable to Modify > Combine the two halves, Body 27 and Body 16 however I am not sure at this moment why. I don't think it is particularly important at this stage.

Both the splines in YZ Cut and XZ cut can now be moved around to better control the result. If they are moved too fay the lofts will likely fail but it should allow you to tweak the behaviour if it is not what you are looking for. If you need the fillet radius to be precise like in the drawing this is very doable, basically creating rails for the two surface loft in steps 9 and 10. I can get into more detail with this if anyone wants but perhaps it would make this all go on for much longer that people have tolerance for.

Please bear in mind that there are better ways to do this and I don't mean to patronise or bore anyone with the details above, I have just attemted to document it in a way which any new Fusion user might be able to follow and reference the screencast.

I hope this helos someone, please feel free to ask if you have any questions.

[beresfordromeo]

I have written some detailed instructions how to address this issue for this user and recorded a screencast. 

The whole thing has taken me the better part of  6 hours to do and for some reason I cannot post it because a moderator thinks I am trying to spam this thread.

I don't post that often for the very reason that I try to get as much detail into my instructions as possible so that they can be followed by absolute beginners.

Could someone please ask the moderators to read my posts before deleting them. I am only lucky that I copied and pasted the text into a sticky so this afternoon has not been a complete waste but I don't know what to do now.

Please help.

[beresfordromeo]

The text I am trying to include in chunks.

------ 
There are several ways that you could approach this and I am sure that others will have plenty to say on that but I thought I would demonstrate a sort of dirty approach. Ideally you would restart the model to properly dictate the parameters of the fillet you want but I think that in order to get you a solution without messing too much with your original sketches this will do for now. Besides the dirty approaches are useful when you inherit designs and need to make changes such as these.

[beresfordromeo]

1 At 0.11 in the screencast I have demonstared a sketch I created on Plane 2 and named YZ Cut; this is on order to cut and prepare the rectangular part Body 15 for better transition to the pipe part.

2. I also created another sketch (see 0.15) called XZ Cut on the XZ Plane for the purpose of cutting the pipe part Body 1.

3. At 0.47 I am showing how I changed the loft that you created for Body 15 to become a New Body rather than a Join. These will keep the two bodies separate so that we can create the transition between them to reflect your design intent, a smooth transition with a variable fillet.

4. At 0.58 I am demonstrating how Body 15 was cut using the spline in YZ Cut, creating a new body (Body 16).

5. Same again at 1.13 but this time cutting the pipe part (Body 1) resulting in a new body (Body 21).

6. At 1.29 I am attempting to demonstrate one of the important details of this method, in order for the loft work I have found it is good practice not to always use a single spline as normal but to use a number of splines to match the feature that you are attempting to loft to. This means that when the cut is made of the Body 1, the resultant body Body 21 will have the number of edges that is required to make the lofting work. Lofting between surfaces with very different geometry works better when the number of edges is equal even if one of the surfaces you are lofting from is a single continuous curve. At 1.37 through to 1.39 I am showing how I achieved this with four splines each tangent to the next rather than using a single spline. I think that this is an important and often overlooked aspect of surface modelling.

7. The upright lines I am showing at 1.50 are to demonstrate how this geometry can be used as a way of viewing and contolling the spline points further down the model so that you can tweak the cuts to make your transition as you would want it to be.

8. At 2.09 I am attempting to show the first loft in the process using lofting in the surface environment. Had I approached this model in a different way this could have been a loft in the Solid environment but this is just a way as I said earlier, there are others and undoubtedly better ways.

[beresfordromeo]

9. If you look at 2.18 you can see that I can only use a tangent profile for Profile 1, the geometry not able to produce an G2 curve because it is too tight in that section, with some extra work however this would be possible. I am pointing this out because this is a common cause of failure for lofts. Sometimes you can get arround this by adjusting the Tangency Weight but perhaps it is better not to get into this for this problem. I will try to demonstrate this one day if I get the chance.

10. The second loft at 2.50 has less strenuous transitions so is able to be G2 between both profiles.

11. At 3.06 I have demonstrated the command to stich these two lofts together to create a surface body, Body 24. Note the tolerance slider is fairly loose here. Sometimes to get a result it is better to perform more than one loft and stich them together rather than persisting with a single loft that keeps failing.

12. .At 3.27 is a straightforward demonstration of the Create > Patch of the back of the body. I don't think I need to detail this except for mentioning that it is a good idea to turn off chaining if your patches are failing and also paying attention in case the edges that you are trying to create include virtually invisible edges that are not obvious but will make any suface loft or patch fail if they are not included in the chain. I am sure this has been the cause of frustration for many beginners.

13. At 4.00 I have shown the use of the combine tool to create a single solid body. This is a useful tool, easy to overlook and I thought worth a mention.

14. The rest of the screencast is a Solid > Create Mirror to create Body 27 from Body 16,  a Create > Extrude.and a Create >Fillet. Nothing comlicated there.

i5 To my shame I was unable to Modify > Combine the two halves, Body 27 and Body 16 however I am not sure at this moment why. I don't think it is particularly important at this stage.
 
Both the splines in YZ Cut and XZ cut can now be moved around to better control the result. If they are moved too far the lofts will likely fail but it should allow you to tweak the behaviour if it is not what you are looking for. If you need the fillet radius to be precise like in the drawing this is very doable, basically creating rails for the two surface loft in steps 9 and 10. I can get into more detail with this if anyone wants but perhaps it would make this all go on for much longer that people have tolerance for.
 
Please bear in mind that there are better ways to do this and I don't mean to patronise or bore anyone with the details above, I have just attemted to document it in a way which any new Fusion user might be able to follow and reference the screencast.
 
I hope this helps someone, please feel free to ask if you have any questions.

[laughingcreek]

primary issue here is the use of loft, which isn't really the right tool for the job.  loft can result in all sort of unintended surface quality issues when linking up multiple non-curvature continuous curves.

first of, the loft isn't tangent across the mirror boundary-

 which results n a near tangent condition at the edge to to be filleted that would cause any fillet to fail-

I THOUGHT changing the condition profile at the center line to directional would solve that.  but it didn't.  I don't understand why, that should be what the setting is for.

so..

dropping back to the old standby of using a helper body (horizon modeling in the new lingo) did improve that situation-

but there is still the problem at the bottom, again caused by the loft.  that's not ever going to fillet either.

I tried removing the fillets in the sketches, and then adding back in modeling space, but again there is something up with the surfaces that won't allow the fillet at the corners to be added back.

The answer of course is to not use loft here. (only use loft when nothing else will do.)

the squarish shape is really just a scaled sweep.  nice thing about using a sweep is you only need the one profile at the mirror line, one path rail, and one guide rail to control the scale.  all the above wonky goes away, and it's easier to execute-

this geometry allows the fillet your after. 

I suppose you could take issue with the fillets at the corners of the original profile also scaling down as the profile sweeps forward. 

if this bother you, you can 

1-delete the fillets after the fact from the solid and apply sold fillets (will work with sweep version, didn't work with loft version)

or

2-remove the fillets from the sketch profiles, and add them in the solid environment. (again, works with sweep version, not with loft version.)

see attached model

[Hend-Eng]

Waw, waw, and waw!

Thanks ever so much for the obscene level of help here - I'm going to need a while to digest all that information. Seriously.

@laughingcreek @beresfordromeo @TrippyLighting @TheCADWhisperer  I'll be back in touch later in the week when I've managed to take all that in, you're all brilliant.

Cheers,

Tom.

[laughingcreek]

Cause I can't leave well enough alone, I'm revisiting this with an update.  I just had something pointed out to me in a different thread And i wanted to see if it effected this model.  low and behold...

so changing nothing but the settings in your loft so profile 1 is set to directional, and DELETING ALL THE RAILS, and making sure tangent rails stays checked (it was before, just sayin, that bits important)-

you now have a tangent condition across the mirror plane, and the edge where the fillet goes is MUCH better.  not as good as with the sweep, but good enough to accept a fillet-

so, the rails where screwing with you and messing the loft up.  If you need to control the curve of the sides more, then you can either add rail at either end of each fillet, or do the sweep function like I suggested before.  still, this is interesting.

with the fillets-

[beresfordromeo]

Hi @Hend-Eng 

I am so sorry that I have messed up your thread with a load of duplicated posts, I have 'reported' them and asked for them to be removed.

Good luck with your project.

[Hend-Eng]

@beresfordromeo Don't worry about it, you espcially have gone way over and above the call of duty!

The thing that confused me about the rails not giving tangent geometry was that the arcs were drawn on centre with the centreline plane. I never realised things could diverge from that initial condition so easily.

In the end I went with changing the loft to a sweep and it's worked from there. I'm super impressed by your dirty tricks bit it's way above my abilities at the moment, I can't evwn begin to get my head around it. I thought I was reaosnable at this game but clearly still a beginner.

How does one do the black and white stripes thing?

Any way to join surfaces that meet at a perfect tangent or along a straight mirror line? No biggie but it would neaten up the look of the thing!

[beresfordromeo]

---

How does one do the black and white stripes thing?

---

You can turn on a Zebra Analysis using  Inspect > Zebra Analysis

The thing that confused me about the rails not giving tangent geometry was that the arcs were drawn on centre with the centreline plane. I never realised things could diverge from that initial condition so easily.

---

I am not sure what you mean here, if this is a question for me let me know which of the steps (number) in the text I wrote you are referring to. Could it be that you are are referencing @laughingcreek's brilliant deduction about the rails in your initial loft? I think this also explains why the combine did not work on my much less elegant solution to your problem, the dirty fix. We should leave @laughingcreek to explain this but I would like to say that there is an important sketching principle particularly for surface modelling that beginners can learn from this.

Thanks again for listening.

[beresfordromeo]

Hi @Hend-Eng 

I am not sure if anyone else has any more to say about this so I hope I am not being rude by adding some information. I think that your model has shown up some problems that probably require some discussion for new users and since it is such a good example of the problem with variable radius fillets I though it worth trying to document these issues.

I have attached a screencast of a workflow for your model that addresses the tangency problems without altering your original sketches, removing the guide rails or changing the workflow too much. This method improves the quality of the surfaces of the model keeps the parameters you sketched and also allows for the variable radius fillet to be used with G2 continuity, that is to say smoother transitions from the pipe Body 1 to the curved extrusion body (I don’t know what else to call it).

1. The first deviation from your workflow occurs at 0.40 in the screencast. I have added a Create > Extrude of Sketch 1. The extrude distance is 1mm though the distance is not relevant, the extrusion must be in the right direction, i.e. opposite to the features being modelled (Y+) creating a New Body (Body 5)

2. The same at 1.15, this is another Create > Extrude, this time of Sketch 3 in the opposite direction to the first (Y-) (Body 6). Again, the distance is unimportant.

3. What steps 1 and 2 do is to create two solids on either side of our loft that can help to give the solver more information about what we want the loft to do. This was the principle problem in my opinion with your original loft, The loft tool can only adhere to the guidance of the rails at the rails, the further the geometry from the rails the less information the tool has to make decisions about how tangent the surfaces are to the perpendicular of the sketch planes (this may require some more explanation for new users).

You touched on this when you said ‘The thing that confused me about the rails not giving tangent geometry was that the arcs were drawn on centre with the centreline plane. I never realised things could diverge from that initial condition so easily.’ The loft tool has to contend also with the other sketch geometry and if you need to maintain perpendiculararity all around the feature it needs this input, hence when @laugingcreek broke the dependency on the rails and used the ‘Direction’ setting this allowed the loft tool to prioritise the planar sketch rather than the rails and hey presto perpendicularity at the planar surface but at the expense of the rails. (I think perpendicularity is also a made-up word).

The way of overcoming this is to use the ‘overbuild’ method and hence the solids created in steps 1 and 2. Actually the one on step 2 should not be necessary since we could theoretically use the sketch plane however that does not always work and I did not want to get bogged down on that point.

4. At 1.53 I have demonstrated how to use the profile of an ‘overbuild’ solid to guide the tangency of a Create > Loft. Because the profile I am lofting from (Body 5) is now a 3D solid and not an infinitely thin planar sketch entity, the loft tool has something to maintain tangency with at its outer edge. This means that the surfaces of the body resulting from the loft (Body 7) can maintain G2 curvature with the side surfaces (the surfaces perpendicular to the profile we used for the loft (Body 5)) as well as using the rails to guide the shape. The end points of the rails are planar to the sketches that created Body 5 and Body 6 and therefore valid inputs to guide the resulting surface. Non planar points are a common cause of failure for loft rails.

For new users wanting to understand the distinction between lofting between sketches, surfaces and solids with G1 or G2 curvature it is worth checking out this short video.

https://www.youtube.com/watch?v=n4NOIPbELBQ

Because we do not need to use Body 5 as anything other than a guide, I have used New Body rather than Join for the Operation field. This is another departure from your original timeline. It seems that you can use either Keep or Merge for the Tangent Edges setting under this scenario, it does not affect the later fillet.

5. At 2.44 I have demonstrated a straightforward Create > Mirror about the Origin XZ Plane.

6. At 3.05 there is a reference to the Modify > Combine of the relevant bodies, the two Extrude bodies, Body 5 and Body 6 are hidden but they could just as easily be deleted at this stage.

7. You can see from the Inspect > Zebra Analysis at 1.15 that there is good curvature continuity between the two combined halves and this should allow the fillet to work through the surfaces created.

This I guess is the point of this screencast and discussion that may help beginners, even if you use proper tangent rails to guide a loft, the tangency may only apply to a surface at or near the rail (which itself is an infinitely thin line). The further from the rail the less likely the rail is to have an impact and the more likely other geometry considerations are going to drive the resultant surface. This is why a fillet, variable or not may work up to a certain radius, but no larger, because the surface it is filleting is not sufficiently tangent at the radius desired.

That is it for the description and motivation behind this screencast. To anyone who already knows this stuff I apologise for the length of this post but as always, I am hoping to document something in a way that new users might be able to get something from, asks questions about or ignore entirely; also for experienced users to tell me I am wrong, being wrong is the only way anyone really learns anything so corrections are not only welcome but desirable.

This was the easy part however and in the next screencast I will attempt to document how I was able to produce the G2 Curvature variable fillet which conforms to your drawing. I think I mentioned on one of my earlier posts this tool is why I would always prefer to use surface modelling for this type of situation. That variable fillet tool is riven with inconsistent and unhelpful behaviours and this model is a great example of how if you can get a handle on them it can be made to work and produce really pleasing results, just don’t try to edit the underlying geometry however….

Anyway, if anyone got to the end of this post, thanks for listening.

 

[beresfordromeo]

 Hi @Hend-Eng 

I am not sure if anyone else has any more to say about this so I hope I am not being rude by adding some information. I think that your model has shown up some problems that probably require some discussion for new users and since it is such a good example of the problem with variable radius fillets I though it worth trying to document these issues.

I have attached a screencast of a workflow for your model that addresses the tangency problems without altering your original sketches, removing the guide rails or changing the workflow too much. This method improves the quality of the surfaces of the model keeps the parameters you sketched and also allows for the variable radius fillet to be used with G2 continuity, that is to say smoother transitions from the pipe Body 1 to the curved extrusion body (I don’t know what else to call it).

Sadly I tried to post this earlier it was deleted by the moderator (probably AI) who thougt it was an attempt to spam this thread so sadly a duplicate will probaly appear again in a couple of days.

I am sorry that I am so useless at posting.

c68c25fb-0837-4699-baa8-b5bc2c4b8013,640,620

[beresfordromeo]

This screencast deals with the fillet part of this problem. I am not a big fan of this tool and this screencast is an attempt to show why and maybe invite experienced users to comment on why I may be using the wrong workflow. Sadly, because this tool struggles so much the video is really long but perhaps that shows how long you have to wait for it to update. It is mildly traumatic because at any time the tool can also crash or hang up Fusion.

1. At 0.05 in the screencast I am attempting to show how the Variable Radius setting on the Modify > Fillet tool works. The arrows that you see are positions on a continuous contour (Tangent Chain) which is formed at the intersection of two geometries (a Create > Sweep and a Create Loft). Also included in this tool instance are two other constant radius fillets, standard stuff.

2. At 0.33 I have edited the earlier Create > Loft in the Timeline, in this case to change the Tangent Edges setting from Merge to Keep.

3. As you can see at 0.40, this makes the fillet fail in such a way as the variable fillet is deleted along with one of the other two fillets. I don’t really understand this but it is not really a huge problem. I guess the geometry has changed and not everything can be parametric but I would be interested to know if anyone else has experienced this behaviour.

4. Having deleted the fillet and restored the loft to its original settings at 1.13,  I have turned off the design history (right-click on base component Do not capture Design History). This is really so that I don’t have to use any processing power to deal with the Timeline.

5. At 1.26 I have created a new Variable Radius fillet using Modify > Fillet, entering four points to control the fillet radius around the continuous curve intersection, ie Tangent Chain is ticked. I have entered a single dimension of 1mm in Point 2 in the tool. There is no point in entering any more information because as you are about to see the tool will fail.

6. Having clicked on OK, if I edit the tool again it becomes apparent that the points have shifted around the Tangent Chain. At this point (2.46) I have deleted the points and added them again into the appropriate boxes. I find that in order for the tool to work in this situation I have to do this. What seems to be happening is that the start and end points of that Tangent Chain, to the fillet tool at least, have changed for some reason. In fact, the points or position could be edited in the dialog box to the right of the fillet size. The following video is a good guide for new users of this tool to get a better understanding of what is happening here.

Autodesk Knowledge Network, Creating Variable Fillets

https://knowledge.autodesk.com/support/fusion-360/learn-explore/caas/video/youtube/lesson/147524-cou...

7. I have found that once these points are edited 2.49, then the point/positions will not change if the tool dialog is closed and re-opened.

8. For this particular model there is a requirement for a 10mm radius fillet at Point 4 (3.30). Once the tool is closed and re-opened (3.59) it has not changed the positions. It is now possible to go on and edit the other positions.

9. I have a entered 13mm for the first of the two points either side of the largest required fillet (30mm), this is in order to make sure that the fillet reduces sufficiently in size before the tightest curvature which would make the fillet fail. What seems to happen is that as the fillet is preview is updated the positions in the tool move around and this can make the tool fail inexplicably. Although I can’t be certain this behaviour is somewhat unpredictable and given the time it can take to produce a failure or result fusion is effectively locked up.

10. At 5.35 I have changed the tool to Curvature (G2). This will also lock up to the tool for some time though I guess this is understandable given the complexity of the task for the tool and the now incorrect position parameters.

11. After a failure at 5.55 I am able to edit the position parameters at 6.23 to get the largest fillet (30mm) into the right position.

12. The variable radius fillet is now complete and although the process is a little traumatic the results are pretty good surfaces.

13. At 8.20 I am able to add more fillets to the same tool instance and complete the geometry. This does show however how long it can take to get this tool to work even if you know what you have to do. For a new user this would be a really frustrating experience.

I am hoping that someone like @jeffstrater (Autodesk)  will be able to comment on whether this is a bug with this tool or just an improper application. It seems like the type of thing that this tool was designed for but it is not for the faint hearted.

Anyway if anyone made it this far thanks for listening and apologies for the duplicated post and the mess it has made of this thread. Sometimes if I post and then edit I get a message saying the post has been deleted as suspected spam only to re-appear some time later. Truly sorry about this.

 

[beresfordromeo]

This is the file with a timeline for this model.