TurboCAD Forums

The Ultimate Resource for TurboCAD Knowledge

Register
 
Be sure your post is relevant to the current discussion.  Create a new topic within the appropriate board if you are unsure.

Cannot Fillet A Part (Made by Lofts)
Read 224 times
* March 25, 2020, 02:21:43 AM
Hello,

I really want to perform some fillets on a part (attached,  part in red).

TurboCAD is not allowing me to perform fillets even if it's as small as 0.5 mm.

I have no  idea what to change to allow it.

Some help would be appreciated.

Regards,
Darren
« Last Edit: March 25, 2020, 02:23:41 AM by dlocke »

Logged
Mostly interested in 3D parts for manufacture, no formal CAD Training; 2D TurboCAD user since yr. 2007.

---TurboCAD: Pro 2016- Pro Platinum
Windows-8.1/64-bit; Intel-Core-i7 CPU; 12GB RAM;DELL AIO


* March 25, 2020, 03:33:27 AM
#1
Maybe you try'd to use 3D fillet from Modify/ Fillet/ Fillet 3D
Try to open 3D Modify toolbar and Fillet Edges from that menu, of Modify/ Fillet Edges

BTW, if your drawing is not like indicated by your signature, please say so, as your signature state v 21, but file was v 2016

Torfinn

Logged
V20, V21, 2015/ 16/ 17/ 18/ 19 Pro. Platinum
Deluxe 2015/ 16/ 19
RedSDK enabled
Windows 10 Home Premium 64 bit, 32 GB
NVIDIA Geforce GTX 780m, 1 GB


* March 25, 2020, 08:56:53 PM
#2
I'm Modify edges, Fillet (not 3d fillet) and it works on all other edges bar the one...See the updated file attached.
I've updated my signature, Thanks Torfinn.

Logged
Mostly interested in 3D parts for manufacture, no formal CAD Training; 2D TurboCAD user since yr. 2007.

---TurboCAD: Pro 2016- Pro Platinum
Windows-8.1/64-bit; Intel-Core-i7 CPU; 12GB RAM;DELL AIO


* March 26, 2020, 01:50:33 AM
#3
I can fillet them all in 1 go with R = 0.5
Maybe you can show in a picture the edge(s) that will not fillet

Torfinn

Logged
V20, V21, 2015/ 16/ 17/ 18/ 19 Pro. Platinum
Deluxe 2015/ 16/ 19
RedSDK enabled
Windows 10 Home Premium 64 bit, 32 GB
NVIDIA Geforce GTX 780m, 1 GB


* March 26, 2020, 02:15:50 AM
#4
Thanks Torfinn... I wish I could do that ... did you perform that on version 2016?

The attached picture shows the edges my 2016 Pro Platinum will not fillet.




Logged
Mostly interested in 3D parts for manufacture, no formal CAD Training; 2D TurboCAD user since yr. 2007.

---TurboCAD: Pro 2016- Pro Platinum
Windows-8.1/64-bit; Intel-Core-i7 CPU; 12GB RAM;DELL AIO


March 26, 2020, 02:59:39 AM
#5

Darren,

select the object (all the little blue squares are displayed).
With the mouse, drag around/across the object to Select all (all the squares are displayed as red).
Then Finish.
It works fine for me.

Logged
Regards Tim

You can design without engineering, but you cannot engineer without design.
Using Win 10 with Designer 2016/2017 and TurboCAD Pro. Plat. 2018/2019 + Lightworks (64-bit versions) + AnimationLab 5.2.
Windows 10 Pro (1909) 64-bit


* March 26, 2020, 03:15:24 AM
#6
I use exact same version and build like you, v 23.2  b 61.2
Did you try to select them all in 1 time ?
And if you dont want them all, deselect the edges you dont want to be fillet by set the R = 0 on them
Or split it so that the plate where there is marks for holes are standing alone, fillet where you want and then add them together again, as i belive that's the culpit.

TC maybe get confused because of the line between the 2 parts ( red ones ), and will not let you fillet them 1 by 1
I just tested that and it was a problem, if i select all i want to fillet at the bottom and do it in 1 go, it did work.

Torfinn

Logged
V20, V21, 2015/ 16/ 17/ 18/ 19 Pro. Platinum
Deluxe 2015/ 16/ 19
RedSDK enabled
Windows 10 Home Premium 64 bit, 32 GB
NVIDIA Geforce GTX 780m, 1 GB


March 26, 2020, 04:09:38 AM
#7
I found a couple edges that will not Fillet.  When either is selected, the operation fails.


Jeff

Logged
TC Pro Platinum 2019, 2018, 2017, 2016 & 2015 (all with LightWorks & RedSDK) & V21
System: i7-5820K @ 3.30GHz, ASRock X99 Extreme4, 16GB DDR4-2133 RAM, Gigabyte GTX 970, Samsung NVMe SSD 950 (256GB), Windows 7 Pro (64-bit) SP1


* March 26, 2020, 04:23:24 AM
#8
Yes, that is the point i believe is the issue, why TC get confused and cant do it, as it is 2 sections on each side at same line.
Assuming the 2 parts have been added together at a point.
If you selct all 5 edges theat should be filleted and do that in 1 time, it should work, select by window or 1 by 1

Torfinn

Logged
V20, V21, 2015/ 16/ 17/ 18/ 19 Pro. Platinum
Deluxe 2015/ 16/ 19
RedSDK enabled
Windows 10 Home Premium 64 bit, 32 GB
NVIDIA Geforce GTX 780m, 1 GB


* March 26, 2020, 09:15:49 AM
#9
I found a couple edges that will not Fillet.  When either is selected, the operation fails.


Jeff

Yup. Then I applied SAT Healing to the part and it filleted OK.

Henry H

Logged


March 26, 2020, 03:18:48 PM
#10
Yup. Then I applied SAT Healing to the part and it filleted OK.

SAT Healing has been very unhelpful to me in the past, so I tend to forget it.  I guess I will have to keep being (mostly) disappointed in it for those times it actually helps.


Jeff

Logged
TC Pro Platinum 2019, 2018, 2017, 2016 & 2015 (all with LightWorks & RedSDK) & V21
System: i7-5820K @ 3.30GHz, ASRock X99 Extreme4, 16GB DDR4-2133 RAM, Gigabyte GTX 970, Samsung NVMe SSD 950 (256GB), Windows 7 Pro (64-bit) SP1


* March 26, 2020, 05:18:22 PM
#11
Thanks All for your time to reply.

Unfortunately for me none of the suggestions worked. SAT, all nodes at once.. I even deleted the 'Built' folder in TurboCAD to get rid of any errors there,...but no avail.

I re-drew the part in a simpler way and performed some fillet. Not what I wanted so going to anti up and buy 2019 Pro Platinum.

Logged
Mostly interested in 3D parts for manufacture, no formal CAD Training; 2D TurboCAD user since yr. 2007.

---TurboCAD: Pro 2016- Pro Platinum
Windows-8.1/64-bit; Intel-Core-i7 CPU; 12GB RAM;DELL AIO


* March 26, 2020, 05:59:28 PM
#12
Thanks All for your time to reply.

Unfortunately for me none of the suggestions worked. SAT, all nodes at once.. I even deleted the 'Built' folder in TurboCAD to get rid of any errors there,...but no avail.

I re-drew the part in a simpler way and performed some fillet. Not what I wanted so going to anti up and buy 2019 Pro Platinum.

SAT Healing worked with your file in v2019; I don't have 2016.

Henry H

Logged


* March 29, 2020, 05:45:36 AM
#13
There are a couple of things about your part  that are causing problems: One is that it's a loft.  It looks like it's intended to be planar-sided, but if you pass a section through the pillar, the sides of the profile aren't linear, they're composed of splines; there's some unintended curvature there, or maybe it's just that ACIS interprets as intended to be not linear/planar because it's a loft.  It's simple to rebuild as an intersect of three polygon profiles, but another workaround is to set fillet offset values a minute increment higher than the radius value.  Filleting often fails because it is more complicated than you might think at corners where more than two faces meet.  Setting the offset value .001 than the radius, I can successfully apply 5.25mm radii with offset values of 5.251.  Doing that, you only have to check three or four of the edges red, the program associates the networked edges with green highlights.  It's a different story if you want to apply different values to different edges; in that case you'd need to vary the inspector bar options, check/uncheck "smooth vertex" and "select smooth sequence", but it's still advisable to apply a small increase to the offsets. 
V2019's got a lot of extra bells and whistles, but I don't think your problem is version-related: I saved your file back to V21 and it fillets to the values I cite with the offsets treated this way. 
« Last Edit: March 29, 2020, 06:06:04 AM by murray dickinson »

Logged


* March 29, 2020, 08:53:40 AM
#14
"...another workaround is to set fillet offset values a minute increment higher than the radius value."

That's an interesting tip, Murray. I hope I can remember it.

Henry H

Logged


* March 29, 2020, 03:44:35 PM
#15
I think that without the increased offset, the fillet surfaces coincide degeneratively at the vertex caps.   Most times TC/ACIS can deal with that, maybe this failure is because the pillar's lofted, and ACIS doesn't see its sides as planes.  The unfold tool will trace all of the part's facets except those two side.  When the part's been SAT healed, this is what unfold sees....

Logged


* March 29, 2020, 06:03:57 PM
#16
I think that without the increased offset, the fillet surfaces coincide degeneratively at the vertex caps.   Most times TC/ACIS can deal with that, maybe this failure is because the pillar's lofted, and ACIS doesn't see its sides as planes.  The unfold tool will trace all of the part's facets except those two side.  When the part's been SAT healed, this is what unfold sees....

May the saints preserve us from that kind of healing.

Henry H

Logged


* March 29, 2020, 07:51:56 PM
#17
Maybe not the healing.  The actual reason why this is such a bear is that the top profile of the pillar isn't a rectangle, it's been slightly skewed somehow, so the loft is twisted and the faces can't be planar.   The diagonals across the top profile are 30.8517987381 mm vs 30.8528880953 mm.  Since the pillar and the piece mounted on it have matched mating faces, it's likely that the upper piece has dodgy geometry too.    The saints can stand down.
« Last Edit: March 29, 2020, 08:02:07 PM by murray dickinson »

Logged