CAD Forum

Hello Guys, i need some help with a super quick problem.

I was trying to create a “cosmetic thread”with the type “Machine thread”, I created the same mechanical piece as my friend, completely identical the only problem is that whenever I click on the edge, “machine thread” type disappears and only lets me choose “straight pipe thread” type.

The main difference is that when he created the piece, he was using a 2021 version of solidworks, while I’m using the 22/23 version.
I think the problem might be in settings:
Tool->Options->Properties->Drafting Standard->Annotations —> APPLY NEW COSMETIC THREAD BEHAVIOR TO NEW PARTS

In my file, this function’s box is ticked and can’t be unticked, in his file it is unticked and can’t be ticked. Every new file I create has this function activated and doesn’t let me change.


Can anyone help?
Thanks in advance

Pics attached are of the Italian version but they’re just to give the idea.

To check/uncheck the "APPLY NEW COSMETIC THREAD BEHAVIOR TO NEW PARTS", you need to open the part template. The option won't be available with a part file active.

You mean creating a new part from zero and, from that part, untoggle the option before clicking on "sketch" to start drawing? Because I tried to create new parts from zero and try to untoggle it but still, it doesn't let me.

In case you meant something different, how do I do that? I'm sorry but I'm a beginner.

No, you need to open the part template. Look for the .prtdot file in your system.

In case you are still unclear, then we can connect online via Anydesk or Teamviewer, and I can show you on your screen.

gupta9665 wrote: ↑Sun Sep 10, 2023 10:03 am No, you need to open the part template. Look for the .prtdot file in your system.

In case you are still unclear, then we can connect online via Anydesk or Teamviewer, and I can show you on your screen.

Ok I'm going crazy, I did what you told me and managed to untoggle but still, I haven't solved the problem. I'll post the 2 files in the attachments. On my file I can't choose Machine type cosmetic thread, on my friend's file I can. Could you take a look when you got time and explain to me why this happens or at least how to solve this? As soon as I click on the edge machine type disappears while it works on my friend's file, both of the holes have the same diameter if you check.

Thanks.

The reason for the issue is that you have used CGS system and your friend's is using MMGS system. This means you part is 10 times bigger and there is no thread size for that size in the database. You can update the database to include that size OR changes your model units (and size as well) to MMGS.

gupta9665 wrote: ↑Mon Sep 11, 2023 1:07 am The reason for the issue is that you have used CGS system and your friend's is using MMGS system. This means you part is 10 times bigger and there is no thread size for that size in the database. You can update the database to include that size OR changes your model units (and size as well) to MMGS.

OMG, I don't know how to thank you, I've been stuck for days on this problem and didn't know Solidworks actualli took into account the units of measurement to any of their processes, I thought it was more of a formal thing.
One last thing, how come do I have to set the diameter lenght to 10,50 to use a M12? I thought it was the hole diameter 12mm, is it the head of the screw instead? Do you know where I can find a table with all of effective dimensions?

Edit: I managed to create the machine thread type but can't visualize the internal thread, differently from my friend. Do you know why?

Edit 2: Solved the problem, it was on option on shaded cosmetic threads. Thanks anyway

PaoloB wrote: ↑Mon Sep 11, 2023 3:31 am OMG, I don't know how to thank you, I've been stuck for days on this problem and didn't know Solidworks actually took into account the units of measurement to any of their processes, I thought it was more of a formal thing.

Glad to hear that all is working now. You need to get your basics clear buddy.

PaoloB wrote: ↑Mon Sep 11, 2023 3:31 am One last thing, how come do I have to set the diameter length to 10,50 to use a M12? I thought it was the hole diameter 12mm, is it the head of the screw instead? Do you know where I can find a table with all of effective dimensions?

Do not use cut extrude for creating holes for the threads. Instead use hole wizard feature to select the thread standard, type, size and other details and SW will automatically create the required hole for you.

PaoloB wrote: ↑Mon Sep 11, 2023 3:31 am ...
One last thing, how come do I have to set the diameter lenght to 10,50 to use a M12? I thought it was the hole diameter 12mm, is it the head of the screw instead? Do you know where I can find a table with all of effective dimensions?
...

The way tapped holes are actually made is to pre-drill a smaller hole, then run a tap into the hole to create the threads.

On an M12 fastener that fits into the hole, the OD of the fastener is 12mm. But the pre drilled hole needs to be smaller than that, or there won't be any material for the threads.

In CAD, the CAD model generally needs to reflect what is going to be manufactured.

You should definitely read up on threads and how they are made.

https://www.starrapid.com/blog/what-eng ... nd-design/
https://en.wikipedia.org/wiki/Threading_(manufacturing)
https://en.wikipedia.org/wiki/Screw_thread

gupta9665 wrote: ↑Mon Sep 11, 2023 7:33 am Glad to hear that all is working now. You need to get your basics clear buddy.



Do not use cut extrude for creating holes for the threads. Instead use hole wizard feature to select the thread standard, type, size and other details and SW will automatically create the required hole for you.

Perfect, thanks for the tip and for your help.

DanPihlaja wrote: ↑Mon Sep 11, 2023 8:12 am

The way tapped holes are actually made is to pre-drill a smaller hole, then run a tap into the hole to create the threads.

On an M12 fastener that fits into the hole, the OD of the fastener is 12mm. But the pre drilled hole needs to be smaller than that, or there won't be any material for the threads.

In CAD, the CAD model generally needs to reflect what is going to be manufactured.

You should definitely read up on threads and how they are made.

https://www.starrapid.com/blog/what-eng ... nd-design/
https://en.wikipedia.org/wiki/Threading_(manufacturing)
https://en.wikipedia.org/wiki/Screw_thread

Thank you, I will definitely take a look

PaoloB wrote: ↑Mon Sep 11, 2023 3:31 am OMG, I don't know how to thank you, I've been stuck for days on this problem

Mr. Deepak Gupta is the man, he's helped a bunch of us over the course of time. The SolidWorks community is lucky to have such a passionate user in it's ranks willing to help people out voluntarily.

Now as a machinist I am just going to state a couple of things that will help most on threads.

1) The solid model doesn't need to have solid threads in the hole and not really even the graphic threads either if you use Hole Wizard and alway select the middle callout that shows the majors dashed circle. Also the feature in the tree show us what you made the hole.

2) the drawing will automatically put the thread callout on the tapped hole or when you use the hole callout detail it puts all the info on that hole and if you made multiple holes in the holewizard it gives to the count of how many.

As Depepak pointed out the units used in the design can cause issues with scertain features and also equations when flipping units of SW files.

Either MM or IN for engineered machined parts, machine use those units only, not feet, meters, centimeters just good old in\mm, use dual units if you need to show both.

Threads and Fits is the hardest things students don't get cause they seem to get skipped over and then either they waist a crapload of time modeling threads when a simple holewize would saffice.

JMO

lenny

PS everyone should own a Machinery Handbook on hand and a drill and tap chart.

Agree 100% with Len_1962, don't show threads unless you have to. Machine shops use the call out to make the threads, all they need is the locations.

I think all designers should program a CNC at least once or make some parts on a manual mill/lathe before doing drawings. You figure out things like tolerance stack ups and why to dimension a certain way pretty quick when your the one having to do it!

TTevolve wrote: ↑Thu Sep 28, 2023 9:45 am
I think all designers should program a CNC at least once or make some parts on a manual mill/lathe before doing drawings. You figure out things like tolerance stack ups and why to dimension a certain way pretty quick when your the one having to do it!

Manual machining really teaches more as you are the "CNC", when students are in the shop and I am showing them how to run a knee mill I tell them I am using LennyCAM

Got one in forum asking how to change drill depth to point of the drill.
So the drill depth will be different for all sized drill and tip angle.

len_1962 wrote: ↑Thu Sep 28, 2023 11:17 am Manual machining really teaches more as you are the "CNC", when students are in the shop and I am showing them how to run a knee mill I tell them I am using LennyCAM

lol, not sure can you even find totally manual machines anymore? ....even our Bridgeport has a controller on it now.

Frederick_Law wrote: ↑Thu Sep 28, 2023 11:44 am Got one in forum asking how to change drill depth to point of the drill.
So the drill depth will be different for all sized drill and tip angle.

maybe because they don't want to punch thru the otherside of the part or just they understand it better or for what they make the hole depth isn't critical

Frederick_Law wrote: ↑Thu Sep 28, 2023 11:44 am Got one in forum asking how to change drill depth to point of the drill.
So the drill depth will be different for all sized drill and tip angle.

In 2023 they added an option within the hole wizard to go to either the drill point end or the transition point like it always has done.

len_1962 wrote: ↑Fri Sep 29, 2023 11:00 am maybe because they don't want to punch thru the otherside of the part or just they understand it better or for what they make the hole depth isn't critical

I see why they want it. Don't know how they'll control it.
Whole shop need same drill
Or drawing specify drill used
Operator will check drawing and use correct drill
All drills need to sharpen correctly.
QC every drill before

When you program a CNC machine your depth on the drill commands goes to the tip point. I assume that is why people wish to see it that way on the prints. I made a chart of all the standard tip point sizes for 82 deg drill bits so our shop guys could add that to the depth on the standard note to get the proper depth for the machine.