STOCK UPDATE FOR THE SECOND OPERATION IN MILLING

[mousongie]

Hi! In Mastercam X6, how can i use the remaining solid of my first operation ( OP 1) as my stock into my second operation (OP 2) where the part have been flipped with a new WCS. Thanks and happy Easter to all.

Similar Threads:

• Need Help!- Milling a profile from outside the stock milling inward towards the center
• Video BobCAD CAM V27 Mill Pro Operation Stock
• Need Help!- Camworks Thread Milling operation
• How to follow the "resulting stock" of the previous operation
• Second Milling Operation at wrong zero...

[cadcam]

if you are using WCS as your planes the stock with follow. now if you use Stock model you can have for example not having to run thru all the 1st ops to run the next ones in Verify. Also stock model in case can be used to machine against.

[seijack]

Actually there are a couple of ways of doing this. You can use a stock model, but stock models still do not support custom tools.

You can however run your simulation in OP 1 > file > save stock > as stl file, in your location.(file in Mcam simulation window) Then go to your backplot/verify options (in the operations manager) select the FILE option > browse to your stl file that you previously saved > select it.. Then when you run verify they next time the stock will look like your OP 1 machining operation.

This is kind of the old way of doing things before the stock model operation was created, but it does work with custom tools of which I have quite a few.

[cadcam]

What do you mean it will not work with custom tool. Maybe if you are talking about rest mill with a custom tool but to do what he want no issues.

[seijack]

Cadcam,

Sorry I have not been on here in a while. If I select an operation that uses one of my custom geometry tools this message appears. I have contacted my reseller and they have told me that the stock model does not support custom geometry tools.

[cadcam]

What version are you running?

[seijack]

We are running the newest rev of X9 of what used to be Mill Level 3 and Solids

[cadcam]

So here is a custom tool and verify I just made up.
As of X9 it is call Mill 3D

[seijack]

Cadcam, Now take that toolpath that you created and copy it to the bottom. Make the toolpath on top part of the stock model. You should get the error that I posted earlier if you created your tool using custom geometry. If not I have made an error creating my tools somehow. Also attach your file so I can show you the issue I am having.

Seijack

[Superman]

Actually there are a couple of ways of doing this.

This is kind of the old way of doing things before the stock model operation was created, but it does work with custom tools of which I have quite a few.

You are correct with both statements......it is an old way......
custom tools should not be used to do surfacing, as the custom shape is NOT actually used for toolpath calculated
( paths are calculated using flatmill, bullnose or ballnose shapes ... ie 12mm cutter that has a R10.6 on the plunge face (like a feedmill tool ), the surfacing op needs to be told it is a 21.2mm ballnose to get the correct path.... you would have the drawing of the actual tool to replicate what would be machined in verify
NOTE....never assume that what is shown in verify is what you end up with....it is only a representation

You do not need to create another machine group to do the 2nd op with a modified stock model, just create another toolpath group for op2

or ( if you have to run op2 using a different machine )
place the insert arrow in the machine group that has the original stock (op1), select the toolpaths, & run Verify.....the stock will not refresh between machine groups

note...., if using a STL file ( that is saved using a fine setting ), will take extended times (or give errors) when calculating toolpaths

[cadcam]

Seijack that cut with the custom tool was the other side the bottom. I did a WCS for the other side op1 and did a pocket and profile and holes. then flipped the part as a new WCS and created this custom tool and faced this side and cut this custom tool. I made a stock model for all the ops on the first side. then used that stock model you see here in the salmon color. Did you need me to make something else up. this not the first time I have done this.

[cadcam]

Superman,
So you know in the new version you now have support for feedmill tool with inserts. you can get the tool profile from the tool vendor and use that profile as your tool and Mastercam will see it. What version you running these days sir?

[Superman]

Superman,
So you know in the new version you now have support for feedmill tool with inserts. you can get the tool profile from the tool vendor and use that profile as your tool and Mastercam will see it. What version you running these days sir?

Hi Jay

currently running X8 ..... X9 is loaded onto the PC's .... but it's trying to find time to configure the network, update posts, instruct others , plus... IT have added extra hurdles....( & I really don't feel like chasing them for the extra headaches that they created ( read this as "blind idiots" ( the their way only mentality ) ), if you get my drift )

My comment was applicable across the version range ( aimed at the X2 - X5 era's ) but would still apply for ALL versions

PS....I never fully trust backplot & verify.....there is still too many things that can be wrong....( especially for the 4/5 axis path transitions )
( & it's easy to remove dots on a screen image, bit different when it is the actual cutter in the material...... harder to put material back on the part )

[seijack]

Seijack that cut with the custom tool was the other side the bottom. I did a WCS for the other side op1 and did a pocket and profile and holes. then flipped the part as a new WCS and created this custom tool and faced this side and cut this custom tool. I made a stock model for all the ops on the first side. then used that stock model you see here in the salmon color. Did you need me to make something else up. this not the first time I have done this.

Cadcam,

Sorry I have been out of the shop. I will try to get something posted in the next few days that will show the issue that I am having with the stock model and the custom profile tools.

[seijack]

So here is a custom tool and verify I just made up.
As of X9 it is call Mill 3D

Cadcam,

Attached is an example of what I was talking about. Tools 1 and 2 have been created using a wire frame I created that I keep stored on my system. Both seem to have been created correctly. Tool 2 was created using the old x4 method using the custom tool ? option. Tool 2 was created today using the X9 Method. If you put tools 1 or 2 in ops 1 and 3 the stock model will not re-generate and give you the attached error. If you use tool 3 it will re-generate because that tool was made in Mastercam by the parameter creation method. The stock model will not allow you to use custom tools using created wire frame geometry.

[cadcam]

Cadcam,

Attached is an example of what I was talking about. Tools 1 and 2 have been created using a wire frame I created that I keep stored on my system. Both seem to have been created correctly. Tool 2 was created using the old x4 method using the custom tool ? option. Tool 2 was created today using the X9 Method. If you put tools 1 or 2 in ops 1 and 3 the stock model will not re-generate and give you the attached error. If you use tool 3 it will re-generate because that tool was made in Mastercam by the parameter creation method. The stock model will not allow you to use custom tools using created wire frame geometry.

Please send mastercam tool file as I cannot refrence the file for this custom tool. is this suppose to be a FeedMill?

[seijack]

Please send mastercam tool file as I cannot refrence the file for this custom tool. is this suppose to be a FeedMill?

Here u go..The .mcx-9 file is the geometry used to create both of tool files. Yes it is a high feed end mill

[cadcam]

OK, So I have found working in both X9 and 2017 it is based on the geo profile. as if I make some small changes at the tip ID of the profile you are using it will work. In 2017 there is a option in creating new tools a now High Feed tools.
So stock model does support custom tools but there are going to be some rules when going to a sharp undercut in the center.

question why are you using control and a point to start at the mid point when cutter Wear and using lead in and out will give what you need.

[seijack]

OK, So I have found working in both X9 and 2017 it is based on the geo profile. as if I make some small changes at the tip ID of the profile you are using it will work. In 2017 there is a option in creating new tools a now High Feed tools
So stock model does support custom tools but there are going to be some rules when going to a sharp undercut in the center.

question why are you using control and a point to start at the mid point when cutter Wear and using lead in and out will give what you need.

Hmmmm. Would you be so kind to attach the X9 file and the corrected tool geometry and tool file. I would like to see specifically where the problem with the tool is. Sounds like it is with the center recessed portion of the geometry that may be causing the issues? I have not downloaded 2017 yet. It looks like they have added tools for high feed cutting. Is there a tool option to use single tooth thread mills? The only thread mills in X9 were multi-tooth thread mills.

Answer: I would normally not use this tool in the fashion that it was used in the posted file. It was simply the easiest/quickest way to illustrate the problem/errors that I have been experiencing trying to use tools created from custom geometry with the stock model option.

[seijack]

OK, So I have found working in both X9 and 2017 it is based on the geo profile. as if I make some small changes at the tip ID of the profile you are using it will work. In 2017 there is a option in creating new tools a now High Feed tools.
So stock model does support custom tools but there are going to be some rules when going to a sharp undercut in the center.

Cadcam, Thanks!!! I was able to get some time to do some testing this morning. I altered the tool geometry from what I was using



to this



I made a new tool and tested it with the file I loaded previously and the stock model works like a charm!!! Thanks for doing the testing on the file that I posted and letting me know what the issue was!!

Seijack