What's new
What's new

Multiple Entity Disorder

NeedForFeed

Plastic
Joined
Jun 29, 2020
Hi guys. I've been using Mastercam 2019 for about a year now and am fairly adept with it, but I've been having issues today that have never come up before. The first is that I am working on 2 levels of a simple part. The only difference between the two is that one level is the front half and the second is the back, and the front end has a groove for a clip ring. I was backplotting my program before writing the operations for the second level, and I noticed that when it switches between my grooving tool & center drill and again between the center drill & drill that it adds 2 entities to that level. There's nothing in the graphics window like any new lines/points or anything, but just going back and forth in backplotting for a couple minutes it added over a hundred new entities. Anyone have any idea what could be causing this?

My second issue began as I was writing my program, while everything was all tickety-boo, and I had like 5 or 6 tools programmed, but when I programmed my drill - which I've done a million times - and backplotted it, my drill came in sideways. Not as in the tool was rotated incorrectly, but like when I was in Top view, the drill came in from it's normal home position, but instead of pointing to the left towards my part it was pointing at me (menacingly). I went through all the menus wherein I created the tool, went into "Setup Tool", checked "Tool Angle", and can't figure out how to unf*ck my drill. The only thing I can see that's out of place is that under "Tool Parameters" where you can set the home position either based on the machine, or user-defined, it say X0,Z0 and won't let me change it. I've changed it a bunch of times on other programs for whatever reason and I know how to, but even when I click on "define" and input my own coordinates, it just doesn't change in the window. When I'm backplotting it appears to come from my normal home position, so normally I'd just chalk it up to just "some strange sh*t" but now I'm thinking it might be related to my sideways drill. Maybe?

Any ideas or suggestions on how to fix any of this would be much appreciated, because like I said, this has never happened to me before (I swear!) and it's really harshing my mellow right now. If you need clarification on something, please ask, because I can sometimes be bad at explaining things. Thanks in advance,

Utterly yours,
- Jordan
 
Have you tried unplugging it and plugging it back in? I'm only half joking. Any time Mastercam starts spazzing out on me like that I close it and reopen it and it has solved all sorts of things.

I'm mostly talking about the phantom entities though. It sounds like you might just have your tool plane wrong for the drill.
 
Yeah, first guess on the drill is a plane.

First guess on the drilling entity creation is a glitch in the matrix.

Can you share a zip2go file?
 
Have you tried unplugging it and plugging it back in? I'm only half joking. Any time Mastercam starts spazzing out on me like that I close it and reopen it and it has solved all sorts of things.

I'm mostly talking about the phantom entities though. It sounds like you might just have your tool plane wrong for the drill.


I actually did do a hard restart on my computer. When that didn't work, I asked a coworker who came and took a look at it and asked if I'd tried turning it off and back on again... Oi vey.

In regards to the tool plane, I looked at my planes tab and there are 3 with green checkmarks next to them: Top, NEW VIEW #1 and NEW VIEW #1-1. I'll admit, I don't know much about planes, but shouldn't there only be one with a checkmark? And why can't I uncheck them? And why can't I delete the ones that I don't want?

First guess on the drilling entity creation is a glitch in the matrix.

Can you share a zip2go file?

Um... probably? Is that different than just a normal Zip file?
 
Not those planes. Inside the toolpath parameters, go down to the planes tab and make sure your tool plane matches up with the one you want.
 
Is it possible you somehow created or otherwise flipped your geometry so that it's running perpendicular to where you should have it oriented?

Are your other toolpaths on that part intact and look okay?

Show us a view in isometric if you can.
 
No plane selection option on lathe drill.

Yep, that's right, I was wrong. My experience with mastercam is 90% on the mill side and it shows. Show us a screenshot of your toolpath parameters and the page for that tool.
 
Drill Toolpath Parameters.jpgdrill info.jpgDrill Toolpath Parameters.jpgPeck Drill Toolpath Parameters.jpgisometric.jpg

Is it possible you somehow created or otherwise flipped your geometry so that it's running perpendicular to where you should have it oriented?

Are your other toolpaths on that part intact and look okay?

Show us a view in isometric if you can.

It's possible, but I didn't do anything differently than every other time that I've programmed a drill, and honestly I'm not even sure how to flip the geometry like that. How would I go about checking that?

I just looked at the other toolpaths, and they all look fine, as far as I can tell. Also, all their home positions seem fine, while this one drill won't change from X0, Z0, and I still don't know if that's related or a separate issue.

Hopefully this isometric view shows you what you were looking for. It's not much.

Show us a screenshot of your toolpath parameters and the page for that tool.

As far as I can tell this all looks hunky-dory, but maybe a fresh set of eyes will see something that I'm missing.
 
View attachment 302072View attachment 302073View attachment 302072View attachment 302074View attachment 302075



It's possible, but I didn't do anything differently than every other time that I've programmed a drill, and honestly I'm not even sure how to flip the geometry like that. How would I go about checking that?

I just looked at the other toolpaths, and they all look fine, as far as I can tell. Also, all their home positions seem fine, while this one drill won't change from X0, Z0, and I still don't know if that's related or a separate issue.

Hopefully this isometric view shows you what you were looking for. It's not much.



As far as I can tell this all looks hunky-dory, but maybe a fresh set of eyes will see something that I'm missing.

In the tool setup page, is the tool set as horizontal or vertical? It's also interesting to me that your tool angle button on your toolpath page is available. That box is greyed out for me. What does it say when you click on that? Does this machine have a B axis?

Edit: Nevermind, forget all that. I see that you're using the default lathe machine and your tool is oriented horizontally. I just recreated all of your settings using the default machine definition and mine comes out fine every time. I tried to purposefully orient the tool wrong and create the path using both the tool setup and the tool angle box and when I do it won't even backplot, it just throws out an internal error.
 
View attachment 302072View attachment 302073View attachment 302072View attachment 302074View attachment 302075



It's possible, but I didn't do anything differently than every other time that I've programmed a drill, and honestly I'm not even sure how to flip the geometry like that. How would I go about checking that?

I just looked at the other toolpaths, and they all look fine, as far as I can tell. Also, all their home positions seem fine, while this one drill won't change from X0, Z0, and I still don't know if that's related or a separate issue.

Hopefully this isometric view shows you what you were looking for. It's not much.



As far as I can tell this all looks hunky-dory, but maybe a fresh set of eyes will see something that I'm missing.

Yeah, now I'm as upside down as you. The geometry thing was a shot in the dark being that everything looked good with how you had your planes.

Everything looks totally kosher to me, and I wouldn't think you could get a lathe drill operation to do that even if you tried. That being said, I haven't frequented Mastercam lathe in about 2 years, so hopefully someone with more recent and in-depth experience will chime in with something I'm missing.

Is the drill actually drilling then top to bottom of how it's oriented in that screenshot, or is it then drilling "sideways" instead of downwards?
 
Just a WAG, but on your tool setup page in the lower left where it says axis combination/spindle orientation, looks like left upper is checked? Can you change it to spindle origin? Or check your other drill toolpaths and see if anything is different.
 
I finally just recreated it. My guess is you had one of those new view planes completely active when you made the path. That's the only way I can get it to do this. Set your active plane to top (like you have now) and make the drill path again. It should come out fine.

The only way I was able to recreate your error was by making an incorrect plane active and then creating the drill op. Mastercam threw a warning up saying that my tool plane wasn't going to match my stock plane, but if you say no to that you can get a horizontal drill to drill incorrectly.

Edit: One suggestion I have for you is to change your tree display to also show the WCS name next to the toolpath name. When you start piling up a bunch of operations, that makes it way easier to diagnose stuff like this.
 
One other thing to try, delete that toolpath and make a new one with same tool, and as ^ he said, make sure top is selected/active when you make the new one. I posted in another thread where my geometry showed 4 chains, but there was a mystery 5th chain not showing up, but the tool was trying to cut it. Had to completely delete the tool path and start over, it basically ignored my "rechain all" in the geometry window.
 
Just a WAG, but on your tool setup page in the lower left where it says axis combination/spindle orientation, looks like left upper is checked? Can you change it to spindle origin? Or check your other drill toolpaths and see if anything is different.

Well I'll be jiggered, I think you got it. axis combination.jpgsilly drilly.jpg

I changed it from left/upper to right/upper and it looks like it fixed it. It even set my home position to X5, Z10, which is where it's supposed to be. That being said, I've never had to change the axis combination before, and I don't even really understand what left/upper or right/upper refers to, and all my other tools in this program and others are always in left/upper, but... it looks like it fixed it.

Can you or anyone explain what's going on here? I'm grateful that it appears to be working, but I'd like to understand what I just did, and why that worked, and why it needed changing just on this one tool.

In any case, thanks to everyone who posted. Maybe this will help someone else with cattywampus tools in the future too.
 
Well, that shouldn't affect the orientation of your tool, but what it might have done is refresh or create a plane which solved it? It could also have just been bugging out, I'm not sure.

The axis combination has to do with the configuration of your machine and shouldn't matter here since you're using the default lathe. Right/left is which spindle you're working on and upper/lower is which turret.

If you look in your planes now, do you have one labelled 'Lathe upper left'?
 
I finally just recreated it. My guess is you had one of those new view planes completely active when you made the path. That's the only way I can get it to do this. Set your active plane to top (like you have now) and make the drill path again. It should come out fine.

The only way I was able to recreate your error was by making an incorrect plane active and then creating the drill op. Mastercam threw a warning up saying that my tool plane wasn't going to match my stock plane, but if you say no to that you can get a horizontal drill to drill incorrectly.

Edit: One suggestion I have for you is to change your tree display to also show the WCS name next to the toolpath name. When you start piling up a bunch of operations, that makes it way easier to diagnose stuff like this.

Man, you had to go deep cuts on that one.
 
Man, you had to go deep cuts on that one.

Exactly my thoughts, and I couldn't be more grateful.

Edit: One suggestion I have for you is to change your tree display to also show the WCS name next to the toolpath name. When you start piling up a bunch of operations, that makes it way easier to diagnose stuff like this.

Good call. I just did that, and oddly enough, that one drill is on a different plane than the others (except for my center drill, which is also on it's own plane), so what I'm inferring from that is that I did fix it in a roundabout way, but I technically should have changed it to NEW VIEW #1, and in theory that would have been the "correct" way to fix it. Is that right?

Tool Planes.jpg
 








 
Back
Top