Actual cut not the same as profile preview

This forum is for general discussion regarding VCarve Pro

Actual cut not the same as profile preview

Postby tjimholte » Thu Nov 09, 2017 7:17 pm

Todays issue...

For some reason the tool path is rounding the corners instead of following the square profile path I programmed. I was able to get the left to cut outs square by changing the start location of the tool path but to run it 4 times just to get square corners is ridiculous.

Anyone had anything like this happen?
Attachments
picture-of-bad-cut.png
RoundCorners.png
tjimholte
 
Posts: 11
Joined: Wed May 31, 2017 10:07 pm
Model of CNC Machine: Shark HD4

Re: Actual cut not the same as profile preview

Postby Adrian » Thu Nov 09, 2017 7:28 pm

Comes up quite often on the forum. Generally it's control software settings (acceleration/declaration) or slop in the machine.
User avatar
Adrian
Vectric Archimage
 
Posts: 7416
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Actual cut not the same as profile preview

Postby tjimholte » Thu Nov 09, 2017 7:32 pm

thanks, I only have 20-30 hours on the machine so I hope its not slop. I'll dig around in the settings.
tjimholte
 
Posts: 11
Joined: Wed May 31, 2017 10:07 pm
Model of CNC Machine: Shark HD4

Re: Actual cut not the same as profile preview

Postby Adrian » Thu Nov 09, 2017 7:42 pm

The other thing to look out for is cutting too fast or deep for what the machine is capable of as well.
User avatar
Adrian
Vectric Archimage
 
Posts: 7416
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Actual cut not the same as profile preview

Postby tjimholte » Thu Nov 09, 2017 7:56 pm

thanks Adrian, I slowed down the feed rate and that resolved the issue. 8)
tjimholte
 
Posts: 11
Joined: Wed May 31, 2017 10:07 pm
Model of CNC Machine: Shark HD4

Re: Actual cut not the same as profile preview

Postby 4DThinker » Fri Nov 10, 2017 5:02 am

G-code G64 and a P parameter can be added to the header area of your post processor to make sure vectors are follow closely (within the value set with P).

Example: G64P.001 will keep the bit within .001 of your vectors.

Example: G64P.1 will let the bit roam up to .1" from the vector in an effort to keep up feed speed.

Without this your machine is rounding off corners so it doesn't have to slow to a stop to turn a corner. Your results were better when you slowed down feed speed, but feed speed could be increased with the G64P.001 command and accuracy can be maintained.
4DThinker
Vectric Wizard
 
Posts: 982
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro


Return to VCarve - General

Who is online

Users browsing this forum: Bing [Bot], Google [Bot], Roly and 12 guests