What's new
What's new

Mastercam Automation

Mattia9793

Plastic
Joined
Mar 24, 2024
Location
Italy
Hi, I've been a Mastercam user for a few years (about 15) I was trying to see if there were other better Cams, but then, I realized that the learning curve would be a very big problem, so I continued with Mastercam. I would like to understand if with Mastercam there is the possibility of having some type of automation. I've definitely never gone in depth with MC so it could be that I'm missing something along the way. I perform different parts from each other, but basically they all use almost the same strategies, so what I notice is that every day I am practically "wasting time" executing the same commands. Does any expert have any suggestions on this? Thanks in advance
 
Not sure if they have any sort of learning functions for milling recognized features similar to NX, but I thought mc has feature recognition for hole making. if you machine a lot of holes, this could be a huge time saver for you.
 
Is there a way to have a parameterized stock model and permanently assign WCS to the stock in MCAM?
You could have an array of operations that identify your stock and part that could be ready to go. Just adjust stock size to your part, drop your model in, align it with the stock and click generate, should at least take care of the 2.5D work for you and hopefully most holes.

This is how I do it in integrated CAD/CAM, not sure if it works when mixing and matching.
 
Not sure if they have any sort of learning functions for milling recognized features similar to NX, but I thought mc has feature recognition for hole making. if you machine a lot of holes, this could be a huge time saver for you.
thanks for the reply, but I mainly do 2D and 3D machining, I do some drilling and threading but no more than 2-3 holes per model.
 
Mi domando, c’è qualche cam là fuori che automatizza i processi? Nella relatà dei fatti, si riesce veramente ad automatizzare? Perché io mi rendo conto che faccio sempre le stesse operazioni, ma ogni modello dovrò andare a selezionare delle Freeform diverse per far fare alla fresa quello che ho intenzione che faccia.
 
Not sure if they have any sort of learning functions for milling recognized features similar to NX, but I thought mc has feature recognition for hole making. if you machine a lot of holes, this could be a huge time saver for you.
MasterCAM does have FBM but it is pretty limited to a few features, I believe some pocketing, contouring and drilling operations but doesn't seem to be very popular amongst users.

From what I've seen NX and CAMWorks are the only two that can really recognize quite a bit of features and be useful. CAM Assist (CAM add in to a few CAM software) looks like it does pretty well from some of the videos I've watched.

@Mattia9793 That might be worth looking into - CloudNC - CAM Assist, they have a MasterCAM add in but I believe its in beta still.
 
There are better cam systems out there and you shouldn't be afraid to try them. Usually you can ask your reseller if they will let you demo the product. Honestly, Mastercam is pretty outdated and overly complicated for the code it produces. The 5-axis toolpaths for example feel totally different because it is literally a totally different piece of software stapled into Mastercam. It also lacks a lot of the more interesting automation features of the new cam software. I am currently working with Mastercam because it is what a lot of people know so it makes it easier to hire people who know it. However, I have used other systems and have seen and experienced how good and how bad other cam systems can be.

To emulate some of the automation of other software packages, I have tried a couple things. Here are some easy ones:

Besides saving toolpath default parameters like in the first reply, I also like to save or return to known sequences and strategies.

This can be done in a few ways, but here are a couple of examples.

I have one Mastercam program I call my "Imperial Threads Master". In the program, I set up individual groups of spot, drill and taps for all imperial thread sizes and then repeated it for plug, sti and roll taps. This way, whenever I see a threaded hole in a program, I can right click to import from that program my toolpaths for that thread type programmed in incremental so I dont have to look at a tap chart or set up any tools etc. I made another for metric.

Using this concept, you can save various templates for known working strategies so you don't have to worry about the problem again. Call these whatever you like and use them the next time you are doing a similar process in a similar material.

Barring creating these templates, you can also look up similar parts and import strategies that way. Keep a list of parts, their size, material and what machine and then you can refer to that the next time you work on something similar.

This is basically what a lot of the "automation" in other cam systems actually is, just a database of toolpath strategies related to specific repeated sequences.
 
Saving toolpath parameter defaults as previously suggested is one way to speed things up.

Saving operation files or importing toolpaths from other programs and reselecting geometry are other methods.
 
Thanks for the advice, honestly when I started my company, (I'm on my own at the moment) I started with Mastercam because it's the cam I know (I used it for 10 years in an average user way). That said after I opened my company I started looking around, and I had approached Powermill Hypermill and Esprit. In the end I had chosen Esprit, however, I quickly realized that the learning would not be immediate, and so I unseated Esprit and went back to Mastercam.

Unfortunately, being on my own, I have to rely on what I know to develop the business, so I realized that now it would be counterproductive to choose another Cam. Keep in mind that my clients give me very tight deliveries, so they order a sample today, and they want it the next day, at this pace you don't have time to stand there and try and try again.

I'm realizing though, that Mastercam is very widespread, but it seems to me a Cam of medium performance.

For example, my main client has 5 Powermill licenses, and I'm told by the guys that they are very comfortable with it.
I am also realizing, that the CAM is as important as the machine.
If the program is poorly done, or not optimized, you can have the best machine in the world, but you will go crazy.
 
I am also realizing, that the CAM is as important as the machine.
What's important with choosing a CAM system is what works for you and your needs, and what you are comfortable with. Everyone can share only their opinions based on their own use and experience, what's "best" for one may not be for everyone. There are plenty of programmers that are incredibly efficient with MasterCAM, using techniques shared above from a few. I personally struggled with MasterCAM.

CAMWorks has just been great for me, the AFR with a dialed in TechDB for me has been incredibly efficient. I can get through some some parts without ever selecting a surface, feature or segment and all my feeds and speeds are there based on material selection. It took me years to actually put time into dialing in everything but I was at where you are, realizing I am just selecting the same features over and over again and wanted to find a way to speed it up, I knew CAMWorks could do it, just needed to make it work for me.
 
If you have Tool Paths that you consistently use... i.e. same tool, same parameters, same machine definition etc. you can simply export your tool groups...

For example, if you have a hole that you spot drill, drill, and tap for a specific feature, you can export that group as a toolpath file. Then, when you have a part that has this feature, you can import it into your tool path and simply reselect your geometry.

This essentially removes having to do repetitive selections for parameters that more or less remain the same.
 
If I am not mistaken, Hypermill and Powermill also have some kind of automation.

Hypermill has the automation module which I don't know how it works

Powermill, on the other hand, has Macros, which seem to work quite well. I don't know how freeform/profile recognition works in this case, though.
 
HyperMill has a few options for automation.

On one hand just basic things like a wizard thats lets you get going faster, like setting your zero and stock.

And it has IMO a very good option for holes, which is the "macro database". You have to do the setup for the database youreslf, but if you invest the time the holes basicly program itsef. To some degree you can also do the same with pockets, but that works just for simple geometries in my expierence.

For my old company i made a database for around 500 types of holes. ø0,4 - 20mm up to 400mm depth with or without threads and up to 5 steps.
Was alot of work and around 4000 individual jobs each with its own ruleset.

But it was such a timesaver, we mainly did parts which where basicly swiss cheese and it didnt matter if there were 200 different holes in them, the whole CAM programm for drilling was made in 5-10min.


I dont know what happend in the last few years in Hypermill, as i dont work with it anymore, but i am sure it didnt stand still.
 
I perform different parts from each other, but basically they all use almost the same strategies, so what I notice is that every day I am practically "wasting time" executing the same commands.
Do you start from scratch each time?

When creating a new part file, I usually open an existing, similar part file to use as a template. Save-as-new, delete all the old geometry, drop in new geometry, reselect geometry for each operation, and delete the operations I don't need. If I need additional operations that aren't in the "template", I'll first try to export/import operations from yet another part file (if available) before creating a new one from scratch.
 
I find a lot of folks struggle with moving from MCAM to Esprit, because you basically have to use features. It's built around feature recognition, and is already doing half of what you want right out of the box.

Esprit is not my favorite software for all things, but if I was looking for automated programming; Esprit TNG (not legacy) would be near the top of my short list.
 
Last edited:
I am far from an expert, only been using mastercam for 2 years, BUT i did come across some interesting features. Pre 2023 can input VB script to automate things.
Here's a link to get you started.
Newer versions switched to C++ and I know very little about that since i'm on 2022, i havent played around with it.
 
Hi, I've been a Mastercam user for a few years (about 15) I was trying to see if there were other better Cams, but then, I realized that the learning curve would be a very big problem, so I continued with Mastercam. I would like to understand if with Mastercam there is the possibility of having some type of automation. I've definitely never gone in depth with MC so it could be that I'm missing something along the way. I perform different parts from each other, but basically they all use almost the same strategies, so what I notice is that every day I am practically "wasting time" executing the same commands. Does any expert have any suggestions on this? Thanks in advance
If you want to continue with MC, you're certainly within your right... But Topsolid has EXACTLY the kind of automation and re-usability of knowledge you want, and it's drag and drop easy.

Forgive the lame background music, but:
 
Do you start from scratch each time?

When creating a new part file, I usually open an existing, similar part file to use as a template. Save-as-new, delete all the old geometry, drop in new geometry, reselect geometry for each operation, and delete the operations I don't need. If I need additional operations that aren't in the "template", I'll first try to export/import operations from yet another part file (if available) before creating a new one from scratch.
I do the same thing, after all most parts look like the ones you did a while back.

Each time i do something unique or tap a new hole i export the cycle to a folder that is organized by tool and by operation. I also have a 999 tool library that each tool I've used has its own number for life.
This is my own way to automate what i can.
 








 
Back
Top