gordsgarage

"Boundary must be closed" warning for 1 of 6 operations

Recommended Posts

Hello all, I am new and this is my first post. 

I am a student learning Mastercam with a purchased copy of camInstructor. I am working with Mastercam2019 and have completed the majority of the 2D mill lessons successfully. However I am stuck on problem that I can't seem to get myself through. It involves slotting each side of a cube. 5 of the 6 sides will slot fine. The 6th side will not regenerate its toolpath and Mastercam displays a boundary warning. I have attached a picture of the part. I have searched the forum archives and found similar posts but nothing that has helped. Details are as follows;

-I complete the courses, step by step, as outlined which includes CADing the part in Mastercam and then running toolpaths

-I am fairly proficient with certain aspects of Fusion360 therefore I redo the Mastercam lessons but instead I use .STEP models that I designed in Fusion360 and import them into Mastercam. They are dimensionally the same as the lesson blueprints

-Currently  I am working with a cube that has a slot on each of it's 6 sides.

--The lesson is teaching me to create 6 planes and then creating toothpaths on each one of those planes.

-When I go to regenerate my left side toolpath it fails and gives me the following warning.  "Boundary must be closed and include two parallel, and straight sides. For example, use Create Rectangle  with Rectangular Shape set to Obround"

-I copy and past the toothpath to each plane. The only change I make in my parameters include rechaining the slot and changing the WCS, T, and C planes.

-When I rechain the slots I am using the face option and select the bottom of each slot as a face.

-5 out of the 6 sides work 100%. I have one side that fails.

-I have rebuilt my model 3 times in Fusion360 and I keep the model as clean as possible using the slot feature. I slot each side identically in Fusion360. I have no overlapping lines or open entities.

-I have attached my .emcam file and my .step file that was create in Fusion 360.

I could continue to outline all the things I have tried to rectify my problem but TBH everything is getting fairly jumbled in my head. Any help, and suggestions, would be greatly appreciated.

 

 

 

MILL-LESSON-WCS-PART-2.emcam

MILL-LESSON-WCS-PART-2-Fusion360.step

Cube.png

Share this post


Link to post
Share on other sites
29 minutes ago, gordsgarage said:

Hello all, I am new and this is my first post. 

I am a student learning Mastercam with a purchased copy of camInstructor. I am working with Mastercam2019 and have completed the majority of the 2D mill lessons successfully. However I am stuck on problem that I can't seem to get myself through. It involves slotting each side of a cube. 5 of the 6 sides will slot fine. The 6th side will not regenerate its toolpath and Mastercam displays a boundary warning. I have attached a picture of the part. I have searched the forum archives and found similar posts but nothing that has helped. Details are as follows;

-I complete the courses, step by step, as outlined which includes CADing the part in Mastercam and then running toolpaths

-I am fairly proficient with certain aspects of Fusion360 therefore I redo the Mastercam lessons but instead I use .STEP models that I designed in Fusion360 and import them into Mastercam. They are dimensionally the same as the lesson blueprints

-Currently  I am working with a cube that has a slot on each of it's 6 sides.

--The lesson is teaching me to create 6 planes and then creating toothpaths on each one of those planes.

-When I go to regenerate my left side toolpath it fails and gives me the following warning.  "Boundary must be closed and include two parallel, and straight sides. For example, use Create Rectangle  with Rectangular Shape set to Obround"

-I copy and past the toothpath to each plane. The only change I make in my parameters include rechaining the slot and changing the WCS, T, and C planes.

-When I rechain the slots I am using the face option and select the bottom of each slot as a face.

-5 out of the 6 sides work 100%. I have one side that fails.

-I have rebuilt my model 3 times in Fusion360 and I keep the model as clean as possible using the slot feature. I slot each side identically in Fusion360. I have no overlapping lines or open entities.

-I have attached my .emcam file and my .step file that was create in Fusion 360.

I could continue to outline all the things I have tried to rectify my problem but TBH everything is getting fairly jumbled in my head. Any help, and suggestions, would be greatly appreciated.

 

 

 

MILL-LESSON-WCS-PART-2.emcam

MILL-LESSON-WCS-PART-2-Fusion360.step

Cube.png

For this error usually :

1> Is your chain a closed chain?

2>Is your geometry aligned with your plane in your operation?

Share this post


Link to post
Share on other sites

Welcome to the forum. Mastercam is a powerful modeler as well so don’t feel like you must model in Fusion. That said your statement of changing WCS, T and C plane throws me off a little bit. I will see if I can explain the WCS process then I will explain the C and Tplanes as best I can to see if this helps you solve your problem. 

WCS is Mastercam is the World Coordinate System and really the heart and soul of any machining. On your CNC machine we can think of this as our Workoffset. Where will be putting he part in the machine to machine. On a 3 Axis machine we have to only think about locating the part in the X Y and Z planes. I will it talk about rotation a this time and we will just focus on 3 Axis processes and methods. If we stand in front of a VMC we can use Left to Right as our X Axis. We can use Front to Back as our Y Axis. We then use up and down as our Z Axis. Sorry just establishing a base of understanding. Now if we took that machine and moved it to somewhere else to machine a part we have just take that machines world coordinate system and changed it from where it was to where it was moved to. In remote machining this is what we do when we set up a remote machining process. We take the machining to the part and not the part to the machine. Our machine if it were capable of moving would then have it’s own left to right, front to back and up and down set of coordinates no matter how we turned it shifted it or moved it as long as we kept it all located an secured then we could in essence machine anything anywhere. How they are able to machine parts on submarines. Hopefully everyone is still following along as there is a point here. In Mastercam the WCS is the how, where and what of the Left to Right, Front to Back and Up and Down to what we are going to be machining. In our example block are we trying to make a program where we are going to handle our part 6 times in 6 setups or 2 time in multiaxis setups. We are going to stick with basics and say 6 setups since we only have a 3 Axis machine. 

Our part doesn’t have to come into our CAM software at the perfect place to work with it. It can come in at any place and angle and we have the ability to align Mastercam with that part to associate what we going to be doing on the machine to what we are going to be machining. That is the job of the WCS to create that association from the CAM to the CNC machine.  We can either move the model to that position or create a WCS where we want on our part to machine it. We are creating our relationship from one to the other. On the block we see here we have to create 6 WCS or position the part in such a way to align it that where all the 6 base planes align it. I have not looked at CamInstructor to know what they teach or recommend. I am going to give you the crazy^millman approach. I would create 6 WCS and I would name the. G54, G55, G56, G57, G58 and yes G59. 🤔Amazing how we have 6 standard offsets on a Fanuc machine and we need to machine 6 sides of a part. I want to teach you to think about work holding and how your going to be machining using the workoffsets on the machine. It also forces you to use the planes manager to assign a workoffset for each WCS by naming each face the workoffset your creating for it. Yes we can cheat and just copy the standard planes and then move then where we need them. I like to use Solid face when creating them. I have had issues with copying planes and find creating them from scratch creates the least amount of issues. In putting your Zero for XYZ think about how your holding the part in a vice. The back jaw is stationary or fixed so that should be your Y position. The top of the stock is easy to pick up and establish so that would be a logical place to Z. X is a personal preference and for left handed people we tend to pick the left side of the part keeping all of our X values X positive. For right hand people it is the right side of the part. Now we establish this and we have made our WCS to work from. We have our Left To Right, Front to Back and Up to Down like we are going to machine it. Now since we are only doing 3 Axis our C and T planes all need to match. When we change the C and T plane in an operation we are saying okay I like who that relationship or placement was established, but I need the CAM to change the relationship of the XYZ to be something different this is what create multiaxis abilities depending on the machine and type of operation. We again are using only 3 Axis so we make sure they are all the same for each of the 6 faces and your process should work correctly. 

When we get into Multiaxis machining then we need to start thinking about the 6 degrees of freedom and which Axis does the machine we are programming for have and what are we going to be machining. That is when the WCS really becomes powerful, because we can have one model and then create our needed WCS for each operation and call it a day. Notice I didn’t say create 6 copies of the model and move them to the Zero. Guess what we have customers we still have to program their part that’s way. One Mastercam file for each operation and move the Part to the Zero. Old School, but if that is what they want then we give them programs the way they want them done. I have taught WCS method and processes to many programmers over the years and once they wrap their brain around the process going back to moving models and creating all that extra work they normally don’t. The lesson looks like a good one and once you see what is creating your issue then it will click and your on to the next thing to learn.

I took Machine Shop in 86 and Mr. Martin handed us a hacksaw and a machinist square. Then he gave us a ruler and said we needed to make a perfect block by cutting off a piece of stock from the length of square stock. Then he gave us a files and sand paper of different grits and said I want a 4 finish when your done and should not be able to see any light through the machinist square when your done on all 6 sides. Took 2 weeks to achieve what he asked, but I did it. It is lessons I still remember to this day. This may seem like a simple exercise your doing, but once you grasp the basics of this then you will see how it all starts to relate to machining and Manufacturing. 

HTH 

  • Like 1

Share this post


Link to post
Share on other sites

Either use Linked edges option under the solid selection or use line/curve (2d geometry) to work around the problem. The fillet in the bottom of the x shaped slot is causing a problem, when it is suppressed it is seems fine.

 

Share this post


Link to post
Share on other sites
8 hours ago, peter ~ said:

For this error usually :

1> Is your chain a closed chain?

When you chain watch where the arrows snap to, if there is a gap in your chain they will move to the gap.

HTH

  • Like 1

Share this post


Link to post
Share on other sites

I'm guessing you're solid chaining...if you picked a Face to chain...

Try rechaining the OP as a loop instead....

 

Call me "old School" but I hate solid chaining, I hate solid chaining, I hate solid chaining

 

  • Like 5

Share this post


Link to post
Share on other sites
1 hour ago, JParis said:

I'm guessing you're solid chaining...if you picked a Face to chain...

Try rechaining the OP as a loop instead....

 

Call me "old School" but I hate solid chaining, I hate solid chaining, I hate solid chaining

 

SOLID chaining and SOLID surface selections are the scourge of the universe IMHO.You cannon even import operations with toolpaths unless you somehow had a SOLID with the same op_idn waiting to grab them in the new file and even then.. Unless you imported the part via nesting then did away with the parent op...but that seems counterintuitive.

Share this post


Link to post
Share on other sites

SOLVED...sort of.

Thanks to everyone for their responses and suggestions. Shout out to 5th Axis CGI for the in depth lesson in WCS, I was able to take away valuable information from it.

Turns out my solution had nothing to do with chaining, levels, or poor geometry. Since I was out of ideas I decided to move the part, and stock, origin. This has solved all of my issues. I attached pictures showing the simply change I made. I did not rechain anything and I did not alter any of my cut parameters. I moved the origin, back and forth, multiple times and confirmed that my 1 boundary would fail consistently in the "fail" location.

The reason this is "sort of" solved is because I don't actually understand why this origin placement caused my issue in the first place.

 

Fail.PNG

Succeed.PNG

Share this post


Link to post
Share on other sites
Quote

Call me "old School" but I hate solid chaining, I hate solid chaining, I hate solid chaining

Me too! I like wire frame chaining. 

Share this post


Link to post
Share on other sites
2 hours ago, The Chipmaker said:

Call me "old School" but I hate solid chaining, I hate solid chaining, I hate solid chaining

For me the derived geometry is worth the extra time as long as you use it to help "tell the story" of the program.

Being able to isolate it also helps chaining or selection process.

  • Like 2

Share this post


Link to post
Share on other sites

I went back to your file and got away from the solid face and use the Loop for that face the toolpath regenerated with no problem. Planes and everything are correct it was the method in which you were picking your geometry was the issue here. Changed that and file is good.

Share this post


Link to post
Share on other sites

Just thought I'd chime in since I might have something to do with that lesson.

The problem is your solid. Without seeing how you modeled it in Fusion, I'd only be guessing but if I remove the feature you're having problems with and remodel in Mastercam, no problems. I can only guess the model in Fusion, that feature is not parallel with the face?? Again, only guessing. Besides, this is a Mastercam course....what are you doing in Fusion :) j/k 

  • Like 2

Share this post


Link to post
Share on other sites
2 minutes ago, mwearne said:

Just thought I'd chime in since I might have something to do with that lesson.

The problem is your solid. Without seeing how you modeled it in Fusion, I'd only be guessing but if I remove the feature you're having problems with and remodel in Mastercam, no problems. I can only guess the model in Fusion, that feature is not parallel with the face?? Again, only guessing. Besides, this is a Mastercam course....what are you doing in Fusion :) j/k 

Agree sir, File and concept were sound good lessons. :thumbsup:

  • Thanks 1

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us