Another Wire Question

[ToolMan184]

Just when I think I have this figured out it bites me in the !@*#$.

 

How do most of you handle the G40 at the end of a contour before it reaches the stop? Here is my problem. When I do a countour Start point, contour, cut point, the last line in the contour has this.

 

N60 G01 Y-.57087

N62 G40 G01 X.19685 <-----Last move to stop point.

N64 M21

 

But my machine is comping for the G40 between the Y-.57087 and the X.19685 which I get a taper. Is there a way to put the G40 after G01 X.19685? I looked in the plineout section which is where it is coming from but if I put it on a line by itself then the starting G41 is on the wrong line. Here is my plineout section:

 

plinout #Output to NC of linear movement - 2D feed

pcantxt1, pbld, n$, sgabsinc, pccomp, *sg20code, pwtcode,

pxout, pyout, pzout, pctype, pwtout, pfrout, strcantext, e$

pwtoutaft

 

If I were using a tab I have been adding an overlap of .002" to make it put the G40 on another line which has worked OK. But in this case Im doing a night burn with 4 parts and want to rough burn all the profiles then do the cut offs in the morning. It seems with MC if you start and stop at the same point and use tabs you can work around things. If you want to start and stop at different points in the contour your basically screwed.

 

Any suggestions?

[edmBosto]

Toolman

quote:

---

If you want to start and stop at different points in the contour your basically screwed.

---

I can only tell you what I am familiar with and hopefully this will help.

To stop at different points with those contours you may need to (change at point)leaving the tab for the morning.

 

This may be what I was pertaining to in another thread as "making a tab with a stop within a tab".

Another option instead of change at point you could also break your geo. and do a partial chain with all your skims on all shapes with zero tabs, and then wire the the remaining in another op using a .030 tab with a stop.

HTH

 

The G40 I would need to look at more in the morning.

[ToolMan184]

Thanks for the info. I will have to look into it later. I had to go back to ESPRIT to get the parts programmed and running. This MC Wire is going to be the death of me. It just seems you have to jump through hoops to get everything to work right. I really want to switch to MC 100% but I just dont have faith in it right now. Luckily the operator caught the taper from the G40 and we only scrapped 1 part. Still cost me about $400 but its better than $1600 for the 4.

 

I had worked on getting this program going for 4 hours in MC, went to ESPRIT and done 2 programs in 30 minutes. But I had to do what I had to do. I just wish CNC would spend some more time on the wire side to make it easier.

[edmBosto]

On the G40...

Can you see this move (taper or dig in with no comp.) in the backplot if you zoom in on it?

Have the operation set to control if it isn't already.

[Guest]

toolman,if you want to send me the file i will take a look at it and try to see whats going on.

[Roger Martin from CNC Software]

quote:

---

I had worked on getting this program going for 4 hours in MC, went to ESPRIT and done 2 programs in 30 minutes. But I had to do what I had to do. I just wish CNC would spend some more time on the wire side to make it easier.

---

I must assume the difference in time/difficulty here is you are familiar to Esprit and not Mastercam Wire (yet).

 

quote:

---

If you want to start and stop at different points in the contour your basically screwed.

---

? Are you trying to leave the slug hanging by the tab and come back and cut it ‘later’?

 

Please send me your file and some explanation of what cutting sequence you are looking for…

Rough with a tab and then cut tab with the final rough and then do finish skims.

or

Rough leaving the tab, come back and cut the tab after and then finish skim.

Etc, etc.

Virtually any operation sequence is possible (and not difficult to achieve - once you know how do it).

[Jerry_P]

What kind of machine are you running. by the M21 code is it a Mits. If so try to radius in and out that will help with your problem.

[ToolMan184]

Thanks Jerry, You may be onto something here. I can see I have to forget everything I know about ESPRIT and get a different mind set for MC.

[Guest]

i don't know anything about mits wire but i don't see how that would change anything.it should cancel the comp on the lead out line after it has completed your contour.toolman,if you don't want to drop the parts,just add a tab and set your max leadout to .020 for contours and tabs.make sure auto cut point is checked.you won't need to create a cut point nor break the geometry.

[Roger Martin from CNC Software]

Point #1 -

Note that in many (most?) cases you do not even need to define a Cut Point. Mastercam knows it needs to lead-off the part the cancel the wire comp.

Note on The Lead in/out parameter page the (as shipped) default state is that ‘Tab Cuts (no dropout method)’ is checked, which forces on the ‘Auto position cut point’ option to be checked.

This really means - Do auto lead-out.

 

Point #2-

The length of the auto lead-out will be (by default) same length as the lead-in move to the chain from the Thread Point. You can override this distance using the ‘Max lead out’ setting on the Lead in/out parameters page.

 

 

So if you place the Cut Point ON your contour and you are using Comp in Control (G40/G41/G42), which 98% of Wire users do, you are going to have problem.

Comp is going to get turned off approaching the Cut Point position and since this move is on your finished part contour = bad part. What this boils down to is – you must have a lead-off , so that the machine is cancelling the wire comp “out in space” and not on your finish part profile. What you are doing if you place Cut Point ON the chain is to override this auto lead-out logic, in effect telling Mastercam not to do any lead-off motion. This is something you definitely do not want to do when using Comp in Control.

[edmBosto]

I myself have never defined a cut point.

Just thought I'd throw that in.

[Guest]

i define one when i want the wire to extend past the endpoint of the contour while cancelling comp,and not lead off perpendicular.

[edmBosto]

I just learned something new today.

Thanks Roger for the laid out explanation, Thanks Del

[Roger Martin from CNC Software]

quote:

---

i define one when i want the wire to extend past the endpoint of the contour while cancelling comp,and not lead off perpendicular.

---

Correct.

You really only need to define a Cut Point when you need to have a specific "ending position".

[ToolMan184]

All of this then you feel like this .

 

Thanks Roger for all your help. I havent had a chance to dig into it yet. Maybe tomorrow I need a beer right now

[deeherk]

+1000 roger..