Incorrect backplot w control comp

[SlaveCam]

I have attached a test file where I use one finishing pass and one spring pass. The first operation does it the "traditional" way, wasting time. To save time, the control compensation is activated only at the beginning and at the end in the second op. Is there some gimmick to make Mcam  backplot this properly?

TEST.mcam

[crazy^millman]

Have your turned on Simulate Control Comp in backplot options? The Explanation Point in the backplot dialog.

[SlaveCam]

Have your turned on Simulate Control Comp in backplot options? The Explanation Point in the backplot dialog.

 

Yes.

[civiceg]

 

 

 Is there some gimmick to make Mcam  backplot this properly?

 

Don't use control comp, wear comp because its not 1980 

[SlaveCam]

Don't use control comp, wear comp because its not 1980 

 

What?! 

[crazy^millman]

Don't know what to tell you. If I do it and backplot with and without I get 2 different results. The fact you are now tells me time to call your dealer and see why your system is not acting correctly.

 

Yes I have not used control comp in 15 years just wear comp.

[SlaveCam]

I use control comp whenever anything of IT8 tolerance or better is required. There's two choices to machining to tolerance:

a. - Change stock to leave value in Mastercam / Repost and save the program to floppy / Take the floppy to the machine / Copy the program from the floppy to memory / Re-select program (okuma control) -OR-

b. - Change tool radius compensation value

Which is faster?

 

The third choice is a new machine but I don't see that happening soon.

[SlaveCam]

Don't know what to tell you. If I do it and backplot with and without I get 2 different results. The fact you are now tells me time to call your dealer and see why your system is not acting correctly.

 

Yes I have not used control comp in 15 years just wear comp.

 

Did you check the test file attached? Do the two operations produce identical backplot results (around the rectangle) when quick verify button is down on your system? 

Because it's 2016 I don't think it's a reason to neglect the control compensation feature... as said above, not everybody use state-of-the-art machines 

[civiceg]

No we use wear compensation. No "full" diameter or radius (depends how the control is set) value gets entered into the control, only the deviation from what it is programmed at and what it cuts at. Typically its zero.

[civiceg]

Control comp, requires more lead in/out. You also can't use the edge corner radius in the contour tool path in Mastercam, while using control comp. So you have to draw your corner radi to break corner edges. 

 

 

Wear comp allows you to interpolate close features with a similar size endmill. Ex. finish milling a .062 hole with a .05 endmill. Wear comp gives you more control over your process end of story.

 

It has nothing to do with state of the art machines. 

[SlaveCam]

OK, I get it now. I've used wear only a couple of times because nobody else in this house use it and it's easy to get confused and thus accidents could happen. But you got a good point there. Getting used to a new and superior process will take some time.

[jeff]

 

b. - Change tool radius compensation value

Which is faster?

 

 

You can't change tool radius comp on your machine if you program with Wear comp? 

In all honesty I don't see a benefit to Control comp over Wear. You still have to comp at the machine to achieve the desired result.

The only difference is the numbers spit out by your post processor.

 

I guess Control comp would help if you have to go from a 1" endmill to a 1/4" endmill, but wouldn't that be a rare occurance?

 

 

Edit, You responded while I was typing this

 

 

Yes, once you get used to Wear, you'll never go back to Control comp.

Good Luck!

[SlaveCam]

Thanks Jeff And apparently the backplot issue is eliminated if using wear comp 

[crazy^millman]

I think you sir have found a bug. When you turn off the enter and exit in the lead in and outs the backplot looks correct. With it on it does not back plot correctly. Having said that the code is correct and where you need to trust your numbers and reality of what will run on the machine than a pretty picture that back plot is all in reality it is. Back plot is just that a pretty picture it is not reality and it is up to you to sort out when you are chasing a real or a false issue. In this case your numbers post out correct and make a good part you move on and get the job done. Report the issue to QC and hope we see a fix for it soon. Since majority of people use wear not sure when or how it will get fixed. When you use the new backplot you still see the same error, but again the NC code is correct so you trust what you know and that is the numbers.

[David Colin]

Here we still have a few machines working with compension in control. Even if some of them would take wear, we decided to stay with control to avoid accident with old programs.

 

AFAIK, any 'wear' toolpath can be converted in 'control'. However I always uncheck 'optimize' as I know what I do and i sometimes don't like how Matercam will optimize my path.

A nice tip (nice bug?): Edge corner radius with control can be used in 2D toolpath even if it's not officially supported.

If you select Computer or Wear to make inputboxes available, you can then enter values. Setting 'Control' back will make values persistent and they will be used for toolpath generation. I don't remember using it in 2017 but it worked with X9.

[Newbeeee™]

Same here.

Wear is undoubtedly the way to go, but legacy programs = accident waiting to happen.

So it's computer comp for everything and control for the tight stuff.

[SlaveCam]

I think control compensation still has use in certain situations. For example, when using grinded endmills for finish profiling. Just measure the endmill and put the value in the control (and make sure the program has enough lead in). Another big one is a grinding tool I measure every time with micrometer before use. Because it's diamonded in the machine eliminating the effect of spindle runout and there is practically no tool deflection, the measured value can be trusted. Of course using indexable cutters wear comp sounds the way to go

[civiceg]

programmed with a .500 diameter endmill--> regrind measures .472

 

wear comp

 

Control set for Diameter

.5-.472= "wear offset"=  -.028

 

Control set for Radius

(.5-.472)/2="wear offset"= -.014

 

You can always use a smaller tool, but using a larger one would require having a large amount of lead in/out, which is back pedaling when talking about cycle times. 

 

However, I would not suggest changing your methods if you have a large program history of control comp programs and you don't want to update. Both methods, should not be in one shop, that is asking for trouble. 

[Newbeeee™]

^^^ coming from a drawing office background and therefore previously not being on machines for years previous, tool compensation REALLY annoys me

Because it's radius and not diameter...

Everyone talks diameter offset but it's radial. I know there's a parameter (talking fanuc) to change it but again historic programs and old ways of working stops me from doing this.

Even the Prototraks have it as diameter, which is what diameter offset is

 

Just like old lathes having to be programmed in radius. WTF!

Who in their right mind says this material is 0.5inch radius?

 

Edit:- I just remembered active reports classed stock as radius for a few releases and I've got a print on my desk at work at the moment where someone has dimentioned the part all in R's.

Straight 2axis turned part with half a dozen diameters on it and all R's...

[jlw™]

Slavecam, your lead in/out looks fine except change it to perpindicular so that it will engage comp in a straight line.