Helix plunge in a pocket roughing

[batraul]

Hello there,

 

My problem is that when I make a pocket roughing and I activate the helix for plunging the helix I get is not tangencial to the toolpath. I mean that the tool enters into the material where it wants and when it have finished making the helix and have reached the step it goes to the center of the pocket in order to start the toolpath creating an abrupt change which is bad for the tool.

 

How can I create an helix which were tangencial to the toolpath?

 

I hope have explain it well.

 

Thanks guys.

[batraul]

sorry, I forgot to tell the MC version. 8.1

[Kenneth Potter]

Yea I get that funky weird stuff too.

 

Turn off the helix entry first

How about Creating another layer then backplot/ save as geometry/ then step slowly thru the backplot to get find the pocket entry point. Then create a point at that location . Delete that unwanted backploted geometry Then add that point to the pocket chain (chain manager} .That will force the pocket tool path to enter at that point. Remember to turn your helix entry back on.

[Guest CNC Apps Guy 1]

Or try this. Create a point a bit above the top of the pocket. When you go to do your toolpath, chain the point FIRST then your pocket chain and it shoud start at the point.

 

JM2C

 

[ 03-29-2002, 10:40 AM: Message edited by: James Meyette ]

[kccadcam]

Is this 2d pocketing or surface rough pocketing??

On materials that are hard on tools I use "Follow Boundry" in Helix,Ramp parameters, seems to work very well.

[batraul]

yeah kccadcam it is surface/rough/pocketing.

 

I've tried this parameter of "follow boundary" but i don't like so much because the tool starts at a point more external and then comes again to the center of the pocket. This makes the tool milling more time with the whole diameter and if you are milling hardened steel the tool will suffer a lot.

[batraul]

Kenneth,

 

Think your idea could be good.

 

I will try but next week. Now, holidays.

[Kenneth Potter]

batraul

 

If you try it out & it works you got to remember this.

 

If you change any tool path pocket stradigies (sp?) you must repeat the steps all over again " move the entry chain point to match the pocket entry point. or if you can Eye it out just move the chained point by translate point to point.

[batraul]

Kenneth,

 

It worked perfect your idea!

Thanks.

[Kenneth Potter]

Glad i can help batraul

 

HEY CNC Folks it would be nice if Mastercam has an option to automaticly link the chain point & toolpath pocket entry locations. Weres the chained point (pre drilled hole for hog Em entry) will always follow the pocket entry (spiral inside to outside ) location if one wants to make minor path /parameter changes. Also make the chain pocket enrty point a different style (eg) "Bulls eye " to alert the programmer that that chained point is linked "welded" to a pocket toolpath.

 

Just A thought

[Ken Erman from CNC Software Inc.]

Version 9 has a new feature that will automatically create drilling operations for a tool to plunge into, instead of having to use Helical or Ramp entry. Once you have created the toolpaths that require a plunge hole you use the Start Hole option. It detects the plunge location and drills holes, it also places the operations in front of the selected operations. Disclaimer: If you change the operation in any way that causes the start point to change in X, Y, or Z you have to delete the drill ops and re-run the Start Hole function, but it is easy to use.

 

PMGuy

[Kenneth Potter]

Thanks Pm guy

 

Version 9 is on my list of things to do !!!!!

going to my resellers work shop on V9 next week !

 

[ 04-05-2002, 06:52 PM: Message edited by: Kenneth Potter ]