AnsweredAssumed Answered

3D sketch strange behavior - Routing

Question asked by Nicolas Duguay on Dec 11, 2020
Latest reply on Dec 15, 2020 by Alex Lachance

Like • Show 2 Likes2
Comment • 31

Greetings,

This problem is eating me a lot of time and giving me a lot a frustrations.

Very often, the 3D sketch I'm working on is going haywire like this for no apparent reason:

(and it can be way worse sometimes)

The shape I'm going for usualy looks like this:

It can happen or not, sometimes, it's ok and sometimes it's not with the same conditions.

It can happen when I'm draging a point or adding a constraint.

It feels like SW 3D sketch code is not very well tuned or I'm not working properly, I don't know...

Also, I can have another problem which gives me headaches (sory for the double question, but it is kind of the same issue). Sometimes, when I'm adding a constraint, even if the sketch is not completely and over-constrainted, I got a red and yellow devil:

I let the assembly I'm working on attached for you to play with, please note I'm working with the routing add-in with custom made components, ("Y-dusting intersection 45° unflanged - Ø24", "dusting-flange" and "dusting pipe unflanged") included in the pack-and-go document, you may have to repair some links since routing can be temperamental.

You can try to constraint the far left bottom segment to 2 inches (which should not be over constrainted if you do) and you should get the red and yellow devil

Thank you in advance for any help!

Attachments

P&G-SW-3D sketch behavior.zip5.0 MB

No one else has this question

Outcomes

31 Replies

1 2FirstPrevious

ömür tokman Dec 12, 2020 2:42 AM
Mark Correct
Correct Answer
Hi Nicolas Duguay
Yes, it can act according to the drawing head when it does not dimension completely in 3d sketch.
There were times I had the second problem. I can't find the reason either.

For this drawing, I think it will be fixed when you delete the tangent command.
Like • Show 1 Like1
Actions
Eddy Alleman Dec 12, 2020 4:41 AM
Mark Correct
Correct Answer
Hi Nicolas,

I played with your assembly and can reproduce your problem.
Then I looked more in detail. I broke all external references because I don't have the surrounding assembly and cannot test using them.

When I "Edit route" I made some changes:
add every end of the 3 end tubes there was a point constraint and I deleted them.
I added a dimension to the first tube to make it similar to the others.
Now I can change all sort of things without getting spaghetti. Just drag the points with the green arrows:
I don't know how those extra constraints got there, but removing them let's the 3Dsketch adapt.
Hope it helps.

Have a nice weekend,

Eddy

PS: the adapted files are attached below.
Attachments
- P&G-SW-3D sketch behavior.zip5.2 MB
Like • Show 3 Likes3
Actions
Nicolas Duguay @ Eddy Alleman on Dec 14, 2020 10:26 AM
Mark Correct
Correct Answer
Hello Eddy, thank you very much for this answer. I think it toss me in the good direction of finding a solution. However, constraining the 3D sketch to an external reference is something very useful for me, those ducting I'm designing always have to end up connected on a machine or an extractor hood in the real world so I'm often modeling them in Solidworks.
That image could be a good example:

In the Pack and Go I layed here, there is a part called "Base" I created for the assembly, it was meant to simulate those attachment points I'm usually using. It seams the assembly didn't find it when you oppened it. It looks like this:

Do you (or someone) think there is a way I can work that allow me to connect those ductings to the machines and avoid the problems I encounter?
Like • Show 1 Like1
Actions
Nicolas Duguay @ ömür tokman on Dec 14, 2020 10:30 AM
Mark Correct
Correct Answer
Interesting, but I'd ratter delete the lenght than the tangency, this constraint is kind of mandatory. The fact that you find it may help understand how solidworks resolve the sketches.
Like • Show 1 Like1
Actions
Eddy Alleman @ Nicolas Duguay on Dec 14, 2020 10:45 AM
Mark Correct
Correct Answer
Hi Nicolas,

I've found you base part in the zip. it was just not included in the assembly. So I added it and constrained it the other way around. Then I could edit route and constrain the ends of the side pipers to the 3 cylinders.

Is that the kind of solution you're looking for? I was just constraining the 3Dsketch to the base part.

Eddy
PS: attached my files below.
Attachments
- P&G-SW-3D sketch behavior.zip9.5 MB
Like • Show 2 Likes2
Actions
Alex Lachance Dec 14, 2020 10:47 AM
Mark Correct
Correct Answer
Sounds very similar to a problem I'm having that is caused by my templates not being up to date.
Like • Show 1 Like1
Actions
Nicolas Duguay @ Eddy Alleman on Dec 14, 2020 11:02 AM
Mark Correct
Correct Answer
Yes, this looks like how I usually work. But when I'm working like that, the problems I'm describing hapens nontheless.
Like • Show 0 Likes0
Actions
Nicolas Duguay @ Alex Lachance on Dec 14, 2020 11:04 AM
Mark Correct
Correct Answer
Ok!
Would there be a protocol I could follow to update my templates? What is there to update?
What and how?
Like • Show 0 Likes0
Actions
Alex Lachance @ Nicolas Duguay on Dec 14, 2020 11:11 AM
Mark Correct
Correct Answer
Existing files have to be recreated or repaired with macros and what not, which does not stop the problem from rehappening eventually.

The templates generated by SolidWorks are supposed to be up to date, but it turns out mine were not, so yours might not be.

How to update:
How to Update Templates in SOLIDWORKS | GoEngineer
File locations:
2019 SOLIDWORKS Help - File Locations Options
Like • Show 3 Likes3
Actions
Nicolas Duguay @ Alex Lachance on Dec 14, 2020 11:13 AM
Mark Correct
Correct Answer
Thank you, I'll look into it and bring back feedback!
Like • Show 1 Like1
Actions
Matt Peneguy @ Nicolas Duguay on Dec 14, 2020 11:52 AM
Mark Correct
Correct Answer
Yep, very well could be your problem:
That part template goes back 20 years.
Read all about it at Crusty Old Template File Gotcha
Like • Show 1 Like1
Actions
Nicolas Duguay @ Alex Lachance on Dec 14, 2020 12:18 PM
Mark Correct
Correct Answer
Alright, my templates was indeed not up to date. It could already be a step in the good way.
I proceeded with the update, but I'm not sure if it is possible to update the template of an already existing part, assembly or drawing. Is it? If so, how?
Like • Show 1 Like1
Actions
Matt Peneguy @ Nicolas Duguay on Dec 14, 2020 12:19 PM
Mark Correct
Correct Answer
Nicolas Duguay wrote:

Alright, my templates was indeed not up to date. It could already be a step in the good way.
I proceeded with the update, but I'm not sure if it is possible to update the template of an already existing part, assembly or drawing. Is it? If so, how?
Unfortunately I don't think you can update the template for existing files.
Like • Show 0 Likes0
Actions
Nicolas Duguay @ Matt Peneguy on Dec 14, 2020 12:25 PM
Mark Correct
Correct Answer
Matt Peneguy a écrit:

Unfortunately I don't think you can update the template for existing files.
There seams to be a complicated way of doing it, a workaround,
https://www.youtube.com/watch?v=pFb3pT7jFMQ
Like • Show 1 Like1
Actions
Matt Peneguy @ Nicolas Duguay on Dec 14, 2020 12:30 PM
Mark Correct
Correct Answer
Nicolas Duguay wrote:

Matt Peneguy a écrit:

Unfortunately I don't think you can update the template for existing files.
There seams to be a complicated way of doing it, a workaround,
https://www.youtube.com/watch?v=pFb3pT7jFMQ
Interesting...I wonder if you could make a macro to automate that? I guess you could do the same with the assemblies.
Like • Show 0 Likes0
Actions
Alex Lachance @ Matt Peneguy on Dec 14, 2020 12:45 PM
Mark Correct
Correct Answer
Not for files that date back to prior to 2018. I was pretty much told all my existing files are screwed.

Unfortunately, it sounds like R&D already addressed this with your SPR escalation, explaining that they would be unable to make any changes to the functionality here for files older than 2018, nor is there a way to convert the legacy data automatically. Since R&D has already addressed this, we are unable to accept this escalation as it would not change the answer we get from the development team

My VAR is looking for a solution to update the template natively, but I haven't heard back from him yet. I'll update back on here when I hear back from him.
Like • Show 2 Likes2
Actions
Matt Peneguy @ Alex Lachance on Dec 14, 2020 1:37 PM
Mark Correct
Correct Answer
Alex Lachance wrote:

Not for files that date back to prior to 2018. I was pretty much told all my existing files are screwed.

Unfortunately, it sounds like R&D already addressed this with your SPR escalation, explaining that they would be unable to make any changes to the functionality here for files older than 2018, nor is there a way to convert the legacy data automatically. Since R&D has already addressed this, we are unable to accept this escalation as it would not change the answer we get from the development team

My VAR is looking for a solution to update the template natively, but I haven't heard back from him yet. I'll update back on here when I hear back from him.
I tried converting a part based on the video Nicolas Duguay posted, and the Part in Part method loses all external references. So, if you are doing anything with reasonable intelligence built in, that method breaks it.
Like • Show 1 Like1
Actions
Nicolas Duguay Dec 14, 2020 3:17 PM
Mark Correct
Correct Answer
Thank you for all the answers.
To this date, I don not have the confirmation if updating the template will resolve my problem, but I will look into it and as soon as I have an answer, I will update the status of this post (or not).
This forum community is a great ressource, thank you very much!
Like • Show 1 Like1
Actions
Alex Lachance @ Matt Peneguy on Dec 14, 2020 4:27 PM
Mark Correct
Correct Answer
Yes, that is the issue that I am facing. I'm lacking in words right now to describe my disbelief.
Like • Show 2 Likes2
Actions
Eddy Alleman @ Nicolas Duguay on Dec 15, 2020 3:27 AM
Mark Correct
Correct Answer
Yes, this looks like how I usually work. But when I'm working like that, the problems I'm describing hapens nontheless.
Hi Nicolas,

Did you experiment with the files I sent you?
I don't have any problems any more after deleting the redundant constraints.

Eddy
Like • Show 1 Like1
Actions
Heiko Sohnholz Dec 15, 2020 5:06 AM
Mark Correct
Correct Answer
Hi,
my advice when working in 3D-(routing)-sketches is to add 2D planes. Maybe in advance, when you now where you want to route, maybe on-demand in your 3D sketch. With a double-click you'll activate these planes and your sketch entities will be 2D "on plane". This will result in much more stable sketches.
And even your example is mostly 2D...
Like • Show 4 Likes4
Actions
Matt Peneguy @ Heiko Sohnholz on Dec 15, 2020 8:12 AM
Mark Correct
Correct Answer
Heiko Sohnholz wrote:

Hi,
my advice when working in 3D-(routing)-sketches is to add 2D planes. Maybe in advance, when you now where you want to route, maybe on-demand in your 3D sketch. With a double-click you'll activate these planes and your sketch entities will be 2D "on plane". This will result in much more stable sketches.
And even your example is mostly 2D...
Just to add on to what Heiko has to say. Don't add too many entities to 3D sketches. Your sketch is fine, but I've seen (and done) much more complicated sketches and they can blow up on you. If you find you need more, add another sketch.
Like • Show 1 Like1
Actions
Nicolas Duguay @ Heiko Sohnholz on Dec 15, 2020 9:01 AM
Mark Correct
Correct Answer
I love it. I'm always looking for good work practices, thank you!
Like • Show 0 Likes0
Actions
Nicolas Duguay @ Eddy Alleman on Dec 15, 2020 9:03 AM
Mark Correct
Correct Answer
I didn't get the time, yet, prety busy at the "office" right now, but, I'll certainly do!
Like • Show 1 Like1
Actions
Alex Lachance Dec 15, 2020 12:59 PM
Mark Correct
Correct Answer
Hey,

My VAR found a work-around that's a little less of a neck pain then the other, altough it still has it's share of pain.

The idea is to correct your templates before doing this.

After your templates are corrected, take existing parts and save them as part templates.
After saving them as part templates, open template and save over part.

Part now exists with correct template, still has correct references also.

Does not work for parts with external references inside them, but it works for every other part.

I hope this helps!
Like • Show 2 Likes2
Actions

3D sketch strange behavior - Routing

Attachments

Outcomes

Attachments

Attachments

Related Content

Recommended Content