Thread Milling - I can't get it working

This forum is for general discussion regarding VCarve Pro
Post Reply
Roelli
Vectric Craftsman
Posts: 181
Joined: Mon Sep 03, 2007 9:10 pm
Location: Germany

Thread Milling - I can't get it working

Post by Roelli »

Hi guys.

Iam trying to make an M8 Thread. (worked great with Vcarve V7 and a gadget)
But I can't get it working with V10.

I tried some different parameters but maybe i misunderstand the settings of the tool.

Any ideas?

Thanks! :wink:
Attachments
Thread Tool.jpg
Vcarve PRO rocks!
...and now it rocks even more: http://paulrowntree.weebly.com/gadgets.html

User avatar
adze_cnc
Vectric Wizard
Posts: 4325
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Thread Milling - I can't get it working

Post by adze_cnc »

What, specifically, doesn't work?

Roelli
Vectric Craftsman
Posts: 181
Joined: Mon Sep 03, 2007 9:10 pm
Location: Germany

Re: Thread Milling - I can't get it working

Post by Roelli »

adze_cnc wrote:
Thu Sep 24, 2020 10:17 pm
What, specifically, doesn't work?
The Screw will not fit into the thread.

Also, when entering the tool parameters I think should be correct the tool barely touches the walls of the core-hole.

I refused the diameter from 4mm to 2mm which looks better now. But „trying things out“ might not be the right way for a precise end result. 🤓

So I guess (and hope) that iam just too stupid to enter the correct values for the tool. Hoping that someone can point me in the right direction.
Vcarve PRO rocks!
...and now it rocks even more: http://paulrowntree.weebly.com/gadgets.html

User avatar
DJ-Bino
Vectric Craftsman
Posts: 112
Joined: Tue Apr 15, 2008 4:34 pm
Model of CNC Machine: Versatil 1800
Location: Germany

Re: Thread Milling - I can't get it working

Post by DJ-Bino »

Hi Frank,

verwende mal folgende Werte für deinen Gewindefräser.
Der Sorotec und Datron funktionieren beide damit.

Die Zahnbreite (S) wird so berechnet D1-D2 /2
Die Zahnhöhe(H) wird automatisch berechnet sobald du die Zahnbreite eingetragen hast.
Du kannst auch die Zahnhöhe(H) nach folgender Formel selber berechnen.
Zahnbreite(S) * tan(Flankenwinkel A /2 ) *2
Den Zahnoffsetwert bestimmst du ja selber. Der sollte die Zahnhöhe(H) / 2 plus ein wenig Aufmaß sein.

Gruß Dieter
Attachments
Gewindewerkzeug Sorotec M5-M10.jpg

Roelli
Vectric Craftsman
Posts: 181
Joined: Mon Sep 03, 2007 9:10 pm
Location: Germany

Re: Thread Milling - I can't get it working

Post by Roelli »

Hallo Dieter,

hab's gerade mal probiert.
Sieht so aus wie auf dem Foto im Anhang.
Die Schneiden vom Gewindefräser berühren die Wände vom Kernloch nur ganz leicht. :o
Attachments
Gewinde1.jpg
Vcarve PRO rocks!
...and now it rocks even more: http://paulrowntree.weebly.com/gadgets.html

User avatar
DJ-Bino
Vectric Craftsman
Posts: 112
Joined: Tue Apr 15, 2008 4:34 pm
Model of CNC Machine: Versatil 1800
Location: Germany

Re: Thread Milling - I can't get it working

Post by DJ-Bino »

Hello Frank,
that's strange. Maybe you can use your file
upload to see if everything is ok.
Hallo Frank,

das ist seltsam. Vielleicht kannst du ja mal deine Datei
hier hoch laden um zu sehen ob da alles in Ordnung ist.

Gruß Dieter

Roelli
Vectric Craftsman
Posts: 181
Joined: Mon Sep 03, 2007 9:10 pm
Location: Germany

Re: Thread Milling - I can't get it working

Post by Roelli »

Klar, hier ist die Datei...
Attachments
M8 Gewinde Test.crv
(72.5 KiB) Downloaded 49 times
Vcarve PRO rocks!
...and now it rocks even more: http://paulrowntree.weebly.com/gadgets.html

User avatar
DJ-Bino
Vectric Craftsman
Posts: 112
Joined: Tue Apr 15, 2008 4:34 pm
Model of CNC Machine: Versatil 1800
Location: Germany

Re: Thread Milling - I can't get it working

Post by DJ-Bino »

Hallo Frank,

du musst den Gewindedurchmesser auswählen, nicht den vom Kernloch.
Deinen Gewindedurchmesser musst du auch mit einem 8mm Durchmesser zeichnen.
Den markierst du dann und wählst aus der Liste M8 aus. Nun kannst du dir auch noch
den Kreis für den Kerndurchmesser des Innengewinde automatisch erstellen lassen.
Der ist bei M8 x 1.25 dann 6.647

Ich hänge dir mal die Tabelle für Metrische ISO-Gewinde an. Da findest du alle Werte.

Gruß Dieter
Attachments
Gewinde Tabelle.pdf
(972.97 KiB) Downloaded 45 times
Frank Gewinde M8x1.25.jpg

Roelli
Vectric Craftsman
Posts: 181
Joined: Mon Sep 03, 2007 9:10 pm
Location: Germany

Re: Thread Milling - I can't get it working

Post by Roelli »

Ah, verstehe.
Hab's mal ausprobiert. Sieht optisch schon besser aus. Aber passen tut die Schraube noch nicht. :?

Ich habe mal die maximale Passungstoleranz (0,328mm) eingestellt und testweise das Kernloch größer gemacht (6,8mm.. weil das auch in Deiner Tabelle als "Kernloch" steht), aber ich kann die Schraube vielleicht so eine halbe Umdrehung eindrehen - mehr nicht.

Vcarve PRO rocks!
...and now it rocks even more: http://paulrowntree.weebly.com/gadgets.html

User avatar
Adrian
Vectric Archimage
Posts: 14544
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Thread Milling - I can't get it working

Post by Adrian »

Is it definitely a 1mm pitch M8 bolt? I know the specifications say that an M8 bolt can only be 1mm pitch but I have M8 bolts in my race car workshop that are 0.75, 1.0 and 1.25.

Roelli
Vectric Craftsman
Posts: 181
Joined: Mon Sep 03, 2007 9:10 pm
Location: Germany

Re: Thread Milling - I can't get it working

Post by Roelli »

Measured with my caliper it looks more 1,25 then any other value.

I just made an M3 thread... and THAT worked! So I need to figure out what's wrong with the M8 thread now.
I measured the parameters of the thread cutter with my caliper and they're different to what the manufacturer says.
Attachments
pitch.jpg
Vcarve PRO rocks!
...and now it rocks even more: http://paulrowntree.weebly.com/gadgets.html

User avatar
DJ-Bino
Vectric Craftsman
Posts: 112
Joined: Tue Apr 15, 2008 4:34 pm
Model of CNC Machine: Versatil 1800
Location: Germany

Re: Thread Milling - I can't get it working

Post by DJ-Bino »

Hello Frank,
Can it be that you cut a left-hand thread instead of a right-hand thread.
I have no problems with the tool parameters and settings.
Hallo Frank,

Kann es sein das du ein Linksgewinde schneidest anstatt eines Rechtsgewinde.
Ich habe mit den Werkzeugparameter und Einstellungen keine Probleme.

Gruß Dieter

Roelli
Vectric Craftsman
Posts: 181
Joined: Mon Sep 03, 2007 9:10 pm
Location: Germany

Re: Thread Milling - I can't get it working

Post by Roelli »

That was the problem. It needs to be right hand of course.
(and it's set to left-hand as default)

It just works completely different from the Gadget (from Paul Rowntree) which I used before.
The old Gadget just uses the center point of any choosen circle and then cuts the thread with the parameter which are adjusted.
Which makes sense to me.

The new, integrated, toolpath needs the Thread diameter (8mm for M8), and nothing else (not the core hole diameter or so).

I work 99% with drawings made by customers. So from now on I always need to check and adjust the diameter of the circles the customers did.

And sadly I always need to set the "D" diameter. It would probably be cooler if vcarve would change it, just as it changes the thread pitch value when choosing another user defined thread.

However, thanks to all for helping me out!
Vcarve PRO rocks!
...and now it rocks even more: http://paulrowntree.weebly.com/gadgets.html

User avatar
DJ-Bino
Vectric Craftsman
Posts: 112
Joined: Tue Apr 15, 2008 4:34 pm
Model of CNC Machine: Versatil 1800
Location: Germany

Re: Thread Milling - I can't get it working

Post by DJ-Bino »

Hello Frank,

Thank you for your reply.
It would be better if the thread direction was preset with right-hand thread.
You don't have to enter the diameter (D) separately.
You just select the diameter in the drawing and then say thread milling.
The diameter is then automatically adopted.
Then you select your thread via user-defined and the pitch (P) is entered automatically.
I think it's actually pretty easy.

Greetings Dieter
Hallo Frank,

vielen Dank für deine Rückmeldung.
Es wäre besser, wenn die Gewinderichtung mit Rechtsgewinde
voreingestellt wäre. Den Durchmesser ( D ) musst du nicht extra eingeben.
Du wählst nur den Durchmesser in der Zeichnung an und sagst dann Gewindefräsen.
Der Durchmesser wird dann automatisch übernommen. Dann wählst du über Benutzerdefiniert
dein Gewinde aus und die Steigung (P) wird automatisch eingetragen.

Eigentlich recht einfach finde ich.

Grüße Dieter

Post Reply