How to Delete Rounds in Solidworks? Cannot get FilletXpert to select the round.

[bnemec]

In Solid Edge there is a direct editing feature called "Delete Rounds" and it works very well IMO. I used it a lot to prep vendor or customer models for other direct edits where all the round faces made a mess. After the direct edits I would just put the rounds back in so they flow the right direction.

I searched "Solidworks delete rounds" and found this help page:
https://help.solidworks.com/2019/englis ... Redirect=1
But it doesn't even let me select the round faces of imported solid. Note these are not crazy surface bodies, I'm working on a clean, water tight parasolid body. Since I'm doing a revision to a part that had already gone through this process in Solid Edge I imported the solid body into SW. It's a good, water tight import, just need to edit it and starting from scratch is much worse option. Instead of just doing the direct edits in Edge and reimport to SW I thought I should try to learn how to do it in SW. After trying for a while I'm left with deleting the faces of the round and then stitching extended faces . I go to the SE model (which started as in import from customer Designer) and the rounds simply delete.

If anyone knows how to do this in SW I would be glad to hear about it.

Attachments are gifs of what I'm trying. On in SW the other in Edge.

[SPerman]

After trying for a while I'm left with deleting the faces of the round and then stitching extended faces . I go to the SE model (which started as in import from customer Designer) and the rounds simply delete.

I typically use Delete Face for doing this. As long as the "Delete and Patch" option is selected, you shouldn't have to stitch anything. Sometimes the geometry is too complex, but 90% percent of the time this works fine for me.

[bnemec]

I typically use Delete Face for doing this. As long as the "Delete and Patch" option is selected, you shouldn't have to stitch anything. Sometimes the geometry is too complex, but 90% percent of the time this works fine for me.

Oh, I should have mentioned SW cannot patch it. If the two rounds didn't converge there near the top I think delete face and patch would work. I've tried selecting about every set of rounds I can think of. It just cannot extend that flat side face up to the top like SE does when using delete face with heal/patch. Just a hunch, but I think SE's Delete Rounds is just Delete Face with a selection filter applied. But there could be more going on in the back ground as it feels more robust than delete face and heal.

[bnemec]

Is there an intersect faces command in SW?

[bnemec]

For this case I just deleted everything then kinda reverse engineered that little dimple that I needed to keep. Cut it in with a couple of drafted cut extrudes and applied rounds.

I'd still like to see better ways of deleting rounds with heal/patch in SW as often times I'm working with shapes that are not easy to model back in with normal parametric features. In those cases I rely on boolean ops on multi-body.

[zxys001]

Delete/Fill can work well you delete in order to preserve faces but if the blend consumes the face, you're scrwd in any tool.

[JSculley]

This is slick and worked for geometry like yours.

[bnemec]

Delete/Fill can work well you delete in order to preserve faces but if the blend consumes the face, you're scrwd in any tool.

For some reason SW cannot patch when I delete that top radius like you showed. Possibly due to 10deg draft on the sides, maybe because the rounds were not created in SW. I don't know. The delete & fill produces some rounded surface.

[zxys001]

For some reason SW cannot patch when I delete that top radius like you showed. Possibly due to 10deg draft on the sides, maybe because the rounds were not created in SW. I don't know. The delete & fill produces some rounded surface.

Without seeing the data, I we don't know either... post a Parasolid x_t?

[bnemec]

This is slick and worked for geometry like yours.

I like that trick they show, I keep forgetting it's available. We learned quick to keep feature works turned off as it doesn't do well with any of our SE2019 models. Nevertheless I turned it back on to try this both ways. It doesn't go like the demo. I need to keep it in mind when models come in from vendors.

[JSculley]

I like that trick they show, I keep forgetting it's available. We learned quick to keep feature works turned off as it doesn't do well with any of our SE2019 models. Nevertheless I turned it back on to try this both ways. It doesn't go like the demo. I need to keep it in mind when models come in from vendors.


image.png

Can you upload the model as a STEP file or cut away the material outside the area of interest, save it out as a STEP file and upload it?

[bnemec]

Without seeing the data, I we don't know either... post a Parasolid x_t?

I would if I could. The screen shots are probably pushing the limits. In this case the base shape to create the dimple is a set of stacked boxes with drafts and fillets so not bad to recreate. Sometimes that's not an option so other tools are needed. I wasn't looking so much for a solution specific to this one isolated case, rather looking to learn the various tools to try in the new system. Which is what is happening here, so very cool and thanks to all.

[Frederick_Law]

Don't try to delete everything in one command.
You'll need to test and try different sequence.
After a while you'll learn which one the delete first.

[bradb]

Don't try to delete everything in one command.
You'll need to test and try different sequence.
After a while you'll learn which one the delete first.

This
I end up having to do it this way alot with imported geometry usually to be able to add draft to a feature. As stated earlier, if the face consumes the radius it probably won't work. I have gone so far as to cut away the area and recreate it. Even that doesn't always work on swoopy parts.

[bnemec]

Don't try to delete everything in one command.
You'll need to test and try different sequence.
After a while you'll learn which one the delete first.

This
I end up having to do it this way alot with imported geometry usually to be able to add draft to a feature. As stated earlier, if the face consumes the radius it probably won't work. I have gone so far as to cut away the area and recreate it. Even that doesn't always work on swoopy parts.

Yes, this applies to any parametric software. As stated earlier, I've tried about every order of delete faces in SW. In Solid Edge the Delete Rounds just works in almost any order. I was checking to see if there's some tool/method in SW that I'm missing. Also as seen in the gifs the face is not consumed by the rounds, I don't know how that got started. The face is there and SE has no problem extending it when the rounds are deleted.

[SPerman]

I think the problem is the two fillets overlapping. That seems to be the geometry that SW can't figure out how to patch.

image.png (23.68 KiB) Viewed 4769 times

[bnemec]

I think the problem is the two fillets overlapping. That seems to be the geometry that SW can't figure out how to patch.

image.png

Yep, exactly. Nothing to patch, the face is there, just need to extend it.

[Frederick_Law]

Try Direct Edit, reduce radius size.

[bnemec]

Try Direct Edit, reduce radius size.

Is that in the FilletXpert? I cannot figure out how to select anything, just says "Please select only face belonging to a fillet or a face with filleted edge(s)."

Maybe because we're still on 2019...

Attached a step and xt of a section of the part.

[Frederick_Law]

Use Inventor:

[Frederick_Law]

Delete fillets at the bottom first.
Then the 3 problem fillets.

[Frederick_Law]

Solidworks direct edit:
https://help.solidworks.com/2023/englis ... _Faces.htm

Delete Face, Move Face.

[bnemec]

Solidworks direct edit:
https://help.solidworks.com/2023/englis ... _Faces.htm

Delete Face, Move Face.

Tried that first, will not patch.

edit: Unless you're saying there's a handy extend and knit faces feature that I'm not finding?
Like this one:
viewtopic.php?p=29461#p29461

[Frederick_Law]

You got me to use SW.
You'll pay for this

I'll be off work till Tue.
Not telling you how it's dome until then

28 faces
28! combinations
Keep trying

[bnemec]

You got me to use SW.
You'll pay for this
DeleteFillets-03.jpg

I'll be off work till Tue.Wed.
Not telling you how it's dome until then

28 faces
28! combinations
Keep trying

LOL. YOU WIN!

[Frederick_Law]

And it's not the same as IV.
I tried that first.

[RichGergely]

I'm having a blast at just deleting faces too, see what happens.

And... I got it to work like Frederick in the end. Initially I didn't think it would work.

Here is the thing though, you need to watch what you are doing. You don't really want to be spending ages trying to delete patch in various combinations and then release it just will never work. You may well of saved a lot of time just trimming/extending instead.

[Frederick_Law]

I'm having a blast at just deleting faces too, see what happens.

It's ok, as long as you don't lose any.

[RichGergely]

It's ok, as long as you don't lose any.

I just saw yours and and thought how did I miss that!! So I redid it. Second effort of delete patch after seeing that you managed it worked.

[bnemec]

It's ok, as long as you don't lose any.

Well poop

Getting closer though. "It can be done" is good motivation.

[bradb]

Here's how I did it. All about order of operation. Only 15 tries.

[zwei]

Maybe i am the odd one here...

For cases like this, where i know what surface i am keeping and the geometry is relatively simple, i just tend to cut away the portion and use multiple replace face

Copy surface

Cut and cut

Replace X4

Personally i try to avoid delete face if possible and feel that delete face take much longer to execute (trial and error, lots of fillets to select, long computation time, etc)