Making Mastercam read G-code?

[khass0410]

So hopefully this is the right spot to post this if not please let me know. So I am curious if there is a way to make Mastercam read g-code and update. I will try and explain the best I can, for instance say you make a program and you want to change something without going back into cad cam to change it, like maybe a G81 drill to a G83 peck drill something simple enough to just type, then you want to open just that section in Mastercam to make sure it looks right. Is there a way of doing this?

 

Hopefully I don't confuse people.

 

[Guest]

Trying to get Mastercam to read the gcode back in after it has been posted is like trying to put a baby back in the womb after it has been birthed, ain't happening.

[Guest MTB Technical Services]

So hopefully this is the right spot to post this if not please let me know. So I am curious if there is a way to make Mastercam read g-code and update. I will try and explain the best I can, for instance say you make a program and you want to change something without going back into cad cam to change it, like maybe a G81 drill to a G83 peck drill something simple enough to just type, then you want to open just that section in Mastercam to make sure it looks right. Is there a way of doing this?

 

Hopefully I don't confuse people.

 

 

There isn't a CAM system on planet earth capable of what you asking for.

[Iulian FILIP]

You can use any text editor to modify the g-code BUT you must be very careful and know what you are doing because you can destroy the machine.

You can try Notepad++(open source) or CIMCOEdit(exists in Mastercam)

[khass0410]

There isn't a CAM system on planet earth capable of what you asking for.

I have a copy to an editor that works with Cadkey that will do this exact thing we are taliking about. Is it something you can buy, no because it was made by a programmer here where I work he made it to do exactly what he wants it to do. But it will only work with like 97 Cadkey.

[khass0410]

Is there not a way to create a chook to make this work? Is it really just that difficult? In our day of time I think the is crucial in big shops that hire programmers that have never even seen a machine. I'm just saying I'd lIke edits to be made be the machinist in the shop, updated by the programmer thru cadcam without having to go into cadcam for every change to see what has bebeen done.

 

Thanks for your responses.

[Guest MTB Technical Services]

Your wrong, and I really really hate telling someone this because I am still a little new to the programming world but I have a copy to an editor for Cadkey that will. Is it something you can buy no because it was made by a programmer here where I work. But again it only will work with like 97 Cadkey.

 

No, You're wrong.

There is not a CAM system on planet earth that can do what you are asking.

Your question and follow up statement about the difficulty of doing what you want,

indicates a profound ignorance of what a CAM system actually is and does.

 

CADKEY was not a CAM system.

You are confusing a scripted output from a CAD system like CADKEY or AUTOCAD with CAM.

A series of PRINT statements in a CDL or Auto-lisp script is not CAM.

I still remember the days when the CADKEY CDL file translator (pronounced CAD EL in the CAM world)

was the most popular translator for getting CADKEY data into Mastercam.

 

NC Code (G-Code) is the last step in the process.

A post-processor, by definition, comes AFTER the work in the CAM is done.

It take the work done in the CAM file and formats the output for a given Machine and Control syntax.

If the CAM system produces G-Code, on the fly, as the operation is defined, then it is using a Code Generator and not a post-processor.

In either case, there is no direct link to the original operation data.

 

Your scripted output from CADKEY is simply storing the actual NC Code with the CADKEY data,

likely in a CDL file itself, thus making it appear that you are actually editing something outside of the system.

What you are actually doing could be accomplished with Notepad.

 

The only systems that can directly do something similar to what you describe are APT command based systems

that allow you to modify, for example, a CYCLE/DRILL command to a CYCLE/DEEP command directly in the CL data.

[khass0410]

No, You're wrong.

CADKEY was not a CAM system.

You are confusing a scripted.

Lol, sorry for saying your wrong, I tries changing my post up but you beat me to it. Anyways I kind of understand now. It seemed that he could do everything + more with Cadkey. Anyways thank you for the brief explanation.

[Guest MTB Technical Services]

Lol, sorry for saying your wrong, I tries changing my post up but you beat me to it. Anyways I kind of understand now. It seemed that he could do everything + more with Cadkey. Anyways thank you for the brief explanation.

 

No apology needed.

 

The key word in your statement is "It seemed that he could do everything + more with Cadkey." is the word seemed.

I can state unequivocally that Mastercam Mill level 1 is light years ahead of what you have previously seen running in CADKEY 97.

 

Based on your questions, I can safely assume that you're doing basic 2D parts.

You should take a good look at the Mastercam FBM functionality.

It can be used to automate the programming of basic 2D holes and features.

I've used it for automatic 5-Axis drilling with great success.

It takes some time to get dialed in the way you need it, but it can be a really useful tool.

 

 

[djstedman]

Just thinking out loud here, but perhaps if the guy at the machine knows more about editing code than the programmer, its time for the programmer and the machinist to switch jobs..

 

Any CNC 'programmer' that can't understand the code that the CAM system is putting out isn't worth having.  The concept you describe is pretty simple, file comes back in after having been edited, programmer opens both files up side by side in cimco using compare, alters Mastercam file to conform with the edited gcode that came back from the floor.

 

This doesn't even touch on the issues that are created for an ISO / AS certified shop if your shop floor guys are editing programs based on what they think is a good idea..

[Colin Gilchrist]

I don't know of anything that would work with Canned Cycles for drilling, but Mastercam V9 had a "reverse post" that would read basic tool motion, and turn it into geometry. It only worked on G0, G1, G2, and G3 moves, so it would't work on anything complicated, but I've used it in the past to reverse engineer the geometry for a part they no longer had the CAM files for. For what it is worth; this process totally sucked. 

 

I agree with what everyone else has said; if you are making edits on the shop floor, bring those edits to your programmer and have them change the Mastercam program to output the correct code. The Mastercam File should be the controlling data for producing your program, and the edits should be made in the correct spot: Mastercam.

[Matthew Hajicek - Singularity]

You can take G-Code and turn it into a wireframe path of where the tool goes.  From that, with some knowledge of the process, one could reverse engineer the part.  It sounds more like what you want though is a verification package.  That is software which will read the G-Code and show you what it will do and what the part will end up looking like.  The good ones are pricey; Vericut and Predator VCNC, and they have to be configured for your machine.  You might get by with NCPlot, which is a backplotter.  It will read G-Code and show you a wireframe path of where the tool will go, and allow you to measure distances and positions.  It understands very complicated code including Macro-B, but it will not show you the cut part.  It can generate a DXF file of the cutter path.

[Newbeeee™]

+1 NCplot - We've reversed a couple of Customers NC files before running it through and saving as a DXF and then into mcam

[khass0410]

Thanks for all the responses. The drilling cycle was nothing but a example, there is a variety of stuff that gets changed day by day.

 

 

Again thanks for all the replies and will def. try and use this information in the future.

[gcode]

Predator VCNC can save Mastercam NCI from a simulation session

Years ago I had about 30 proven Cinci 3X gantry mill files we needed to run on a Fanuc

I ran them through Predator, saved the NCI then ran that through our V9 Fanuc post.

The results were pretty good.

The files were 95% milling and it translated really well.

I don't recall how the drilling came out.

I think it was close but some careful hand editing was required.

[jlw™]

Just thinking out loud here, but perhaps if the guy at the machine knows more about editing code than the programmer, its time for the programmer and the machinist to switch jobs..

 

Any CNC 'programmer' that can't understand the code that the CAM system is putting out isn't worth having. The concept you describe is pretty simple, file comes back in after having been edited, programmer opens both files up side by side in cimco using compare, alters Mastercam file to conform with the edited gcode that came back from the floor.

 

This doesn't even touch on the issues that are created for an ISO / AS certified shop if your shop floor guys are editing programs based on what they think is a good idea..

Ditto that. Nothing beats years of experience.

 

As far as changes, every machinist is different. Every one has preferences. I try to keep in mind what machine and who is running it when I create tool paths. No matter how clean and smooth your program is, some one will want something different.

 

Here's how I lead when I hand some one a thumb drive (it makes the operator/machinist feel involved and that input is not shunned but requested):

 

Number 1, first part is on me. The rest of them are on you.

 

Number 2, take notes and let me know what we can make better.

 

Having put my time in, I know the experience on the floor is valuable.

 

Everything is in the approach!

[Gracjan aka Pullo]

You should never say never!

 

 Somebody said here that there isn't a cam system on the planet that can do it (the feature is bi-directionality). Well there is . it's called WINCAM . 

 

http://www.camtek.fi/en/wincam-software/postprocessors-and-simulators

 

Gracjan

[Guest]

You should never say never!

 

 Somebody said here that there isn't a cam system on the planet that can do it (the feature is bi-directionality). Well there is . it's called WINCAM . 

 

http://www.camtek.fi/en/wincam-software/postprocessors-and-simulators

 

Gracjan

 

If I read that correctly, it only offers what Cimco, NCplot and a few others do...it can backplot your gcode and allow a saved dxf....

 

The original question was "Can it update your operation in operations in Mastercam"  The answer to that is still a resounding no.....

 

No gcode can be read an the read back in and actually update Mastercam operations

 

[Guest MTB Technical Services]

You should never say never!

 

 Somebody said here that there isn't a cam system on the planet that can do it (the feature is bi-directionality). Well there is . it's called WINCAM . 

 

http://www.camtek.fi/en/wincam-software/postprocessors-and-simulators

 

Gracjan

 

 

No, this is NOT doing what the original poster asked.

 

If you had actually read what was posted you would know this.

 

There is no CAM system on planet earth that allows you to change the posted output

and have that output automatically updated in the CAM system operation.

If you believe there is, you smoke crack.

[YoDoug®]

In order to accomplish what the OP was asking is a tall order. You would most likely need a custom post that outputs a lot of comment is the NC code. Comments for what operation number, post blocks, etc. Then you would need to have a Chook that reads the posted code and the shop floor modified code, scans for differences, identifies which operations and portions are different by the comments, and then uses a very complex algorithm to decide if it can translate the code changes back into the original Mastercam toolpath settings available. The time and effort to develop this would be far greater than the benefit of having it. 

[gcode]

You should never say never!

 

 Somebody said here that there isn't a cam system on the planet that can do it (the feature is bi-directionality). Well there is . it's called WINCAM . 

 

http://www.camtek.fi/en/wincam-software/postprocessors-and-simulators

 

Gracjan

As stated earlier, no software can turn g-code into a Mastercam file

Camteck looks like it can do a little more than just create  DXF wireframe though.

It can create a model of the machined part.

I'm guessing you give it tool definitions and initial stock size and it simulates the

removal of stock.

That could be useful in some circumstances

[DanielGingras]

Let's keep the personal attacks to a minimum. We can disagree without insulting those we disagree with.

[Jayson Kramer]

Gcode, truthfully this does not help much as if you wrote in MC and go back in and change to a peck cycle and repost is so much less work then dicking around trying to bring what you all ready did in the first place back in to make the change.

 

If your files are organized were you do not have hunt and peck to find the file. it really on takes a few min at most to pull a file back up and toggle using the example of drill to peck cycle change.

I do not see any advantages to this whole thought of what is being asked.

 

Just my opinion. sorry.

[Mick]

I guess it could be done with enough work. Maybe. But then, maybe not.

 

I haven't checked out the Camtek link above (I'm sitting in a Vericut class at the moment ), but something like that, combine with what I can see in Topsolid (Topsolid displays a window of g-code that is updated as the operations are created/changed).

 

But, as JParis and MTB have stated, so far, as any of us know, there is no CAM system that provides a direct link to the NC code and updates the toolpath/geometry file.

 

Yeah, thinking about it, there are ton of variables that come into play

[Newbeeee™]

ENHANCEMENT REQUEST!!!!!!