No Retract on Depth Cuts

[Rick McAllister]

Hello All,

I'm experiencing a little problem with retracting between depth cuts. I'm cutting some 304SST and need to retract between depth cuts to clear chips. I turned "Keep Tool Down" off, set my retract height at .5 absolute with top of stock at 0 abs. "Use Clearnce Only..." is off. The path does not retract between depth cuts in backplot which I verified with posted code. The only way I've been able to accomplish the retract is by setting Depth Cuts to "by Contour" which is not efficient in this case. This problem occured in a newly created program on a differant P/C also. We have not installed the 9.1 Service Pack on our system yet ("if it's not broke don't fix it") but we have all the current patches installed. Is anyone else having this problem?

[David Colin]

I think I had this problem before with closed chains 2D contour. Lead in/out with arcs saved me.

 

Check you didn't checked 'use only clearance on start/end of operation'

 

[ 07-31-2003, 11:42 AM: Message edited by: David Colin ]

[Rick McAllister]

David,

I'm leading on and off with arcs but still damaging cutters. Use clearance.... is not checked. Thanks anyway.

[David Colin]

Did you (just to try) to select compensation control by computer?

 

I'm still pretty sure i had this problem before... I did a similar toolpath yesterday and it worked with V9.1 (I'll try V9.0 tomorrow)

[Thad]

Rick,

 

Can you post the file to cadcam's ftp?

 

Thad

[crazy^millman]

If you are doing holes you need to not do manual pick items you need to go to the entities and pick the item from there. If you are doing contours then you need to go to a retract distance that is atleast .100 higher than your strat plane. good luck.

[Rick McAllister]

Thad,

I dropped it on the FTP site. I didn't know I wouldn't be able to move it once it was there so it's on the root directory. Perhaps Cadcam would be kind enough to move it to the MC9 folder. Sorry Cadcam, just call me green. I named it NO RETRACT.MC9 and santitized all non relevant operations. Play with it and let me know if you find a solution.

 

THX

[McRae]

Rick,

 

If chip evacuation between depth cuts is the concern, then I might suggest that you use "Pocket" and then add a point chain in front of the circle chain for all of your elements. This did the trick for me on a new tool path.

 

See the FTP on Pocket_Andrew_Retract.MC9 (in the proper folder though...)

[Rick McAllister]

I'm finishing three diams, .688, .625, .645, with a 1/2" end mill 1.20" dp. Holes are predrilled with a 15.5mm (.610) drill thru. I don't think changing the type of toolpath will help. All I need is Mcam to retract between depth cuts and it's not working.

[Rick McAllister]

Could this be a post issue?

[McRae]

No this isn't a post issue, the tool path simply doesn't do what you want. I changed to something valid that would give the intended result. As the holes are drilled out already, this makes it more attractive to use the pocket solution. With the material at the center of the cutter already removed, the plunge is that much less of an issue.

 

quote:

---

All I need is Mcam to retract between depth cuts and it's not working.

---

This is because the function that you want is not iside of the contour tool path. Different type of a scan you see. Besides - it takes 30 minutes to talk about it and only 5 minutes to make the changes, copy the geometry into the new tool paths, post the code and cut the part.

 

Using a Pocket Tool Path will even allow a finish pass at the final depth to size - which is desirable for the 4 place tolerances that it looks like you are trying to achieve (although I would only ever bore/ream/burninsh something that fine...)

 

[ 07-31-2003, 03:25 PM: Message edited by: Andrew McRae ]

[Rick McAllister]

Andrew,

Here's the sinerio: I have a family of parts previousely programmed. I don't have the time to go back and recreate all those paths in all the programs and repost and reproof. I don't mean to seem impatient but the "Keep Tool Down" function in "Depth Cuts" is not working as it should. The tool is staying down regardless of the radio buttons selection. It used to work prior to V9.1.

[McRae]

quote:

---

the "Keep Tool Down" function in "Depth Cuts" is not working as it should. The tool is staying down regardless of the radio buttons selection. It used to work prior to V9.1.

---

Scope of the problem is now further understood. Please send to qc@mastercam and maybe they can offer a solution. I wonder if the logic for the Keep Tool Down is buggered in the MC source code now if it worked in previous releases...

[crazy^millman]

I did take your part and do A circle toolpath using entites instead on manual and it did retract on me. It may have worked before but if that does what you want for now it could help cut your cycle time and do the chip clearence that you want. Just a thought good luck and full understand the time crunch thing good luck.

 

Crazy Millman

[Rick McAllister]

Thanks for your time guys.

I think I'm going to have to come up wth plan B like 'change at point' (if this will work).

 

Thanks agian.

[iowajim62]

Hi Rick,

 

Was wondering if you still have 8.1.1 or 9.0 installed ? If so have you tried with them ?

[Rick McAllister]

Jim,

Got rid of the old versions. Mcam kept opening new programs with old versions. File associativity problem in XP.

[Rick McAllister]

Solution:

Because the point of entry and point of exit are exactly the same the cutter WILL NOT retract regardless of "Keep Tool Down" selection. I don't like this feature and now have to go back and change the entry point on every program and every operation that needs a retract just to clear chips. Perhaps CNC Solutions should reevaluate this function. Normally I prefer to have bores start and end at the center of the arc which gives the operator a point he can use if he needs to troubleshoot.

[8sigma]

I found this thread when I was having the exact same issue on MC 2020.

I'm using the center of the hole for entry and retract.

I deselected the "use exit point" on the lead in/out tab and set a perpendicular lead out to get the cutter off the wall.

I deselected "keep tool down" on the depth cut tab, and selected "keep tool down" on the Multi Passes tab.

The tool retracts after each depth for clearing chips.

[jeff]

Wow digging up a thread that is over 16 years old. That's impressive.

[crazy^millman]

1 hour ago, 8sigma said:

I found this thread when I was having the exact same issue on MC 2020.

I'm using the center of the hole for entry and retract.

I deselected the "use exit point" on the lead in/out tab and set a perpendicular lead out to get the cutter off the wall.

I deselected "keep tool down" on the depth cut tab, and selected "keep tool down" on the Multi Passes tab.

The tool retracts after each depth for clearing chips.

Throw a sample file together showing your issue and share it so we can play along. Over 15 years ago I helped and still helping those who need it. 

[nickbe10]

This could be a post issue ...

[JParis]

Just now, nickbe10 said:

This could be a post  poster issue ...

fissed

[nickbe10]

On 1/3/2020 at 12:20 PM, JParis said:

fissed

Who was it that said:

  "Every time I think I am getting too cynical, I stop and think about it for a few seconds and realize I am just not keeping up..." ?

 

[8sigma]

On 1/3/2020 at 12:03 PM, 8sigma said:

I found this thread when I was having the exact same issue on MC 2020.

I'm using the center of the hole for entry and retract.

I deselected the "use exit point" on the lead in/out tab and set a perpendicular lead out to get the cutter off the wall.

I deselected "keep tool down" on the depth cut tab, and selected "keep tool down" on the Multi Passes tab.

The tool retracts after each depth for clearing chips.

 

On 1/3/2020 at 1:53 PM, 5th Axis CGI said:

Throw a sample file together showing your issue and share it so we can play along. Over 15 years ago I helped and still helping those who need it. 

I made some screenshots for the benefit of those not running MC2020. 

Geometry: select the point at the center of the hole, then the contour.

Depth cuts: UNCHECK "Keep Tool Down"

Lead-in: use entry point

Lead out: NO EXIT POINT. Very important. use a perpendicular exit less than the center distance.

Multi-Passes: CHECK "Keep Tool Down"

Linking: Make your clearance high enough to clear the chips. 

               UNCHECK "Use clearance only at start and end..."

These settings will retract to the clearance plane at the end of each depth level. Press single block as it comes up and blow out the chips.

Alternatively I suppose you could create a sequence at each depth if you needed program stops.

HTH, Steve.