Mill Guy Thrown to Lathe Wolves

[Rotary Ninja]

Thanks. Our reseller actually sent us a modified post. I figured it was an easy flip switch.

[Rotary Ninja]

Ok, so my programs post out with V values which alarm the machine out since it is just a 2X Lathe. Can this 4X post be edited easily enough to omit these V values?

 

Edit:
I see in the post I see...

y_axis_mch : 0 #SET_BY_MD - Machine has a Y axis, 0=no, 1=yes - Set based on Axis Combination in MD

 

Does that mean I will need to modify the machine def to get rid of this?

 

Edit #2:

I did just that and it is fixed. Did I do this right? I created a new 2X Machine definition then I deleted the right spindle and the Y-axis on the turret. It posts out correctly now. So I just want to make sure I didn't do something I wasn't supposed to do.

 

Thanks

[Rocketmachinist]

Go into your machine definition and take out the y axis.

[Rotary Ninja]

Yeah, just did that. Thanks for the confirmation. I also have the Machine definition using the 2X control definition. Everything seems to be posting out the way it needs to now.

[Rocketmachinist]

The one other things I would check to see if you post it right.

 

A threading cycle for some reason had an E for feed instead of F.

 

Drilling cycles had a G98 which swaps the machine to ipm instead of ipr.

 

I brought the feedrate roundoff to 6 decimal places.

 

I had my initial rapid and retracts to do Z first and then x so it won't get into trouble with the tailstock. The sl30 would error if it tried to go strait to the that point because of the safety boundary.

[Rotary Ninja]

Ok, you have exceeded my technical ability at this point. Our Haas Lathe is a limited edition. Meaning we don't have live tooling LOL. So far the worst I have to program are grooves. When I get to threading I will look you up!

[Pilot Plant Supervisor]

Our Haas lathes work fine with the E for federate. The IPR or IPM for drilling cycles can be switched in the toolpath manager on the page where the feed and speed are entered.

[Rocketmachinist]

I always had it set to ipr and it would still throw out the ipm even though it didn't need it and when you are trying to drill at .003 ipm there isn't a whole lot going on.

[Rotary Ninja]

Ok. I am programming a face groove. The OD of the groove is a tight diameter and the machinist wants to touch off of the OD of the tool. I understand his thinking so I got to looking and I cannot see a way to change which side of the groove tool you are compensating to. Is there a way to change this? Other than lying to MasterCam and telling it is the opposite hand tool I mean.

 

Thanks.

[K2csq7]

Custom tool......

And grooving is not for the faint of heart. 

Send the file over and I'll take a crack at it. 

 

If you NEED to get the job done NOW, I suggest telling your operator "that's just how it is", shift the tool offset the width of the insert and run it. If you have the time I'll PM you my work email. 

[K2csq7]

Your PM box is full I guess... shoot it to

 

K2CSQ7

 

hotmail.com

[Rotary Ninja]

I was guessing it would have to be a custom tool. Why can't there be a simple check box?

 

Anyway, I cheated and used a different hand tool and got it. It works just fine, it just backplots the tool holder backwards, which isn't an issue. I will delve into this deeper when I have more time.

Thanks.

[Rotary Ninja]

We have noticed that the final retract moves aren't clear of the part sometimes before the machine is sent to home. Luckily the machinist running the job is keen on this and has caught it every time. How do I tell MasterCam to pull straight out to a safe position (like Z+.250") before sending the tool home?

 

Thanks.

[Rocketmachinist]

Reference point

[K2csq7]

We have noticed that the final retract moves aren't clear of the part sometimes before the machine is sent to home. Luckily the machinist running the job is keen on this and has caught it every time. How do I tell MasterCam to pull straight out to a safe position (like Z+.250") before sending the tool home?

 

Thanks.

 

Mr. Ninja, 

 

If you have a file this happens in.... Please send it in to QC!!!

[Colin Gilchrist]

If you program you part without defining "Stock", Mastercam will not retract out of a bore fully, to provide adequate clearance before going to the tool change position.

 

If you define "Stock" in the Machine Group Properties, Stock Setup page, prior to programming your tool paths, then the "Tool Clearance" setting should get used to make sure the tool is positioned "outside the stock" before retracting. (I think the default clearance value is .03).

 

That said, I've had this "feature" not work before when programming lathe parts. For that reason, I do like Rocketmachinist recommended and I always use an "Approach" and a "Retract"  Reference Point.

 

Using Reference Points for ID work is the best way to prevent a crash in Mastercam Lathe. I tell everyone I train how to use this feature...

[Rotary Ninja]

Ok, I have messed with Reference Point. Is there a science to it? Or do you just select user defined and pick a point somewhere in space that looks safe?

 

Thanks guys.

[Colin Gilchrist]

Hi Kevin,

 

Reference Points are a feature that is included in every Lathe toolpath. It isn't something you set once and forget. I'm not sure what you mean by "user defined". I think you might be using "home position"?

 

Here is how I usually set mine for I.D. work:

 

Notice that I set "Z" only, and force the position to Absolute, so I can be 100% certain that the tool retracts to that Z value before it goes home to the Tool Change.

 

BTW, I think you can use the "Coordinates" button (left and down from "Ref point") to setup where the tool change location is, relative to your XZ zero. That way it shows the tool approaching/retracting to the correct location when you backplot/verify.

[Rotary Ninja]

Ahh, there is the devil I was looking for!

 

Thanks!

[Rocketmachinist]

Reference point is a must for when I am running my tl1 with gang tooling. Each tool might look like it will feed in correctly and cut the part the way you want, but if when you transition from one tool to another there can be some nasty crashes.

[Newbeeee™]

Kev  -use ref points for retracts for indexing on Rotary Work as well - you can control the tool to go where you want it before a toolchange so long milling type tools (remember them ) don't thwak the 4th axis on toolchanges.

Oh milling's easier than turning isn't it?

[Rotary Ninja]

I have used reference points a lot in milling for just such occasions. I just didn't see that grayed out check box down there until I saw the screeny here. My machinist thanks you guys too. More to come

[CADCAM3D5AXIS]

Hi Kev

as said above ref points will save $$$$ when it come to id work and od.  But you must make sure each tool has it turned on  for every tool and it is set for the tool you are checking . I always just go .100 on the od and .100 off the face  and the id  i set it to -.05 from the smallest bore   and .100 off the face that way your rapids   will work for you when you have long b bars stuffed down a bore.  i check them every time  before posting just to make sure.  also watch your lead in and lead out settings cuz they will add to the pucker factor.

HTH  

[Rotary Ninja]

Thanks. I am starting to get comfortable programming the lathe. I got an attaboy for a beautiful part we just pulled off. Grooves and all looked very good. I am impressed with how easy it is to program a lathe part and how well MasterCam is at generating a toolpath that really works well.

 

They are talking about getting a large VTL. I was dreading programming a lathe. Now I am actually looking forward to getting that big guy in here. It's really quite fun!

[Newbeeee™]

Thanks. I am starting to get comfortable programming the lathe. I got an attaboy for a beautiful part we just pulled off. Grooves and all looked very good. I am impressed with how easy it is to program a lathe part and how well MasterCam is at generating a toolpath that really works well.

 

They are talking about getting a large VTL. I was dreading programming a lathe. Now I am actually looking forward to getting that big guy in here. It's really quite fun!

I found the biggest thing is that lathes are all about clearances.

While you're watching through the window the tool cutting with feed override down, what you should be watching is the adjacent boring bar that's just about to be wiped out but the chuck jaws ROR!