Esprit 2020 to Mastercam 2022

[Shiva.aero]

Hello everyone! I am new to this forum and this is my first post!

I am a user of Esprit 2019 CAM for 5 axis programming of Aerospace components. Recently my employer decided to shift to Mastercam 2022 (because of some commercial policy issue over SMC) and placed the purchase order for Mastercam 2022.

I searched this forum and some other sites regarding the advantage and disadvantage of Mastercam over Esprit CAM.  I got some useful answers but all are old post (before 2012).  So here are some of my questions / doubts:

1. Many points out that Mastercam post needs editing and it is not robust like Esprit. Is it still the case or improved? (I never had any problem with Esprit post and I never heard anything like post edit other post customisation for requirement)

2. Esprit have a "5 axis channel roughing" operation, which is Multiaxis trochoidal roughing operation between 2 walls. We use this operation for roughing of Impellers and Blisks. In my quick search in youtube and Google, I couldn't find any equivalent tool in Mastercam. Is there any equivalent tool for trochoidal roughing of Impellers and Blisks in Mastercam 2022?

3. The two main problems I faced with Esprit are 'Axis limit control' and 'External rapid links'.

Some critical 5 axis operation like the one in mentioned in point no.2 does not have axis limit control and the tool axis is directly derived from geometry edges, which results in the frequent problem of tool path exceeds axis limit problem.

It is very 'very' difficult to create collision free internal and external rapid links'. You need to spend hours to get a collision free rapid links'.

Are these cases same with Mastercam? Or will I be free from these problems?

4. With Esprit we tried to customize the post processor for 'LOOPS'. That is instead of extracting NC code for each individual features of a pattern, only one program will be extracted and it will be looped using macro. This we got it done for 3 axis but couldn't get it for 5 axis. I explained this to our Mastercam reseller and they told they will try but not sure about it.

Is this really possible with Mastercam post?

5. What I shouldn't miss asking my reseller? Is there any important technical documentation that needs to be asked from reseller?

6. Esprit conducts 'Esprit World conference' every year. It's a great knowledge sharing platform. Is there anything similar for Mastercam?

7. Any tips or books to deeply understand Mastercam?

Happy to join this BIG forum! (never heard of such forum for any other software)

Curious to learn Mastercam.

Thank you.

 

 

 

[gcode]

Hello

You don't say what machine(s) you require posts for

It sounds like you are doing advanced 5X work

I recommend you check out the official Mastercam forum 

You will need to create an account to access this forum

The account must be created on a PC with a Mastercam license on it

Advanced Solutions for Manufacturing | Mastercam

Mastercam has a free generic 5X post you can download from the Tech Exchange

Tech Exchange - Home (mastercam.com)

This will require lots of editing and is not recommended for a new user. 

There are also hundreds of sample part files and tutorials 

available on the tech exchange.

Mastercam also has machine/control specific posts available for purchase

Post Processors - Mastercam

There are a wide variety of online courses available

Learning Tools | Mastercam Support

The owners of this forum sell a wide range of books and tutorial for Mastercam

as well as posts.

eMastercam Store

Post Request - eMastercam.com

 

Postability | Mastercam Post Processors

My employer has more that a dozen Postability posts and I cannot recommend them highly enough.

From personal experience I know Postability will be happy to provide you with a trial license  

You will have to go through your Mastercam dealer to purchase any of these posts.

As for Mastercam's 5 axis capabilities.

Mastercam licenses the Module Works 5 axis module

https://www.moduleworks.com/?jet_download=10576 

(the port and multiblade modules are available for Mastercam as options)

It can do 5 axis trochoidal roughing  between vane walls with collision avoidance 

and axial limit controls with the miltiblade options

 

Welcome to the forum. 

 

 

 

 

 

 

 

[Colin Gilchrist]

If you do a lot of Blade Roughing and Finishing, you should speak with your Reseller about Moduleworks Blade Expert. This is an add-on program to Mastercam, specifically for roughing and finishing Blades. It takes hours of work, and turns it into minutes or seconds. Enter a few parameters, select the blade geometry, and the Toolpath algorithm does the rest.

Mastercam has 5X roughing with Dynamic (Mastercam's word for Trochodial, or controlled radial engagement paths). However, the Blade Expert goes far beyond just Dynamic style cutting.

There are several tools for dealing with rapid links between Operations. Some of that will depend on which paths are being linked together. Blade Expert will link flawlessly with other Moduleworks paths. Sometimes you might need Multi-axis Link, but that path has been going through some revisions lately. I haven't investigated the capabilities in a while. With Mastercam, you can always use a Point Toolpath, or Curve 5-Axis, to manually link paths together. 

Posts work great if you purchase a good one, and are available through your Reseller, and also 3rd party Post Developers exist and are very good. Look to Postability or In-House Solutions for a Post for your machine. Unless you have a Mill-Turn, then you will need a Mill-Turn Machine and License from CNC Software.

LOOPS are known in Mastercam as Subroutines. There are many options for using Subroutines in 3-Axis, but not with 5-Axis, that I'm aware of. I've done some on my own, by using a G52 shift to "temporarily shift the Zero Point", and then repeating a 5-Axis Subroutine, but this is much easier on a Gantry machine. Toolpath Transform can be used on 5-Axis paths, but not necessarily for Subroutine output. However for nesting Operations on a tombstone, or just several parts in a row, Toolpath Transform can be used to output Subroutine calls with new Work Offsets. So you can repeat the same program at G54, G55, G56, Etc.

 

[Shiva.aero]

Thank you gcode & Colin Gilchrist!

1.

 You don't say what machine(s) you require posts 

The machine is DMG mori DMU70 5 axis milling machine  with Siemens 840d controller.

2. We ordered Blade expert. But our reseller told that it doesn't support dynamic roughing. They informed that it may be possible using a tool called 'Multiaxis Pocketing' and they are yet to confirm.

3.

17 hours ago, Colin Gilchrist said:

However, the Blade Expert goes far beyond just Dynamic style cutting

We machine hard materials like Wasploy, Udimet, Nimonic-90, etc., Traditional roughing never worked out on these materials. Does 'Blade expert' offer any superior method than Trochoidal/Dynamic milling?

4. Manual linking using point option will be great.

5. I was not knowing about 3rd party posts! We ordered with Mastercam for the post. Thanks for the information.

6. 3 axis loop/subroutine is an easier one and I have written some code on my own, which works without any problem. But, 5 axis with RTCP mode is difficult. I attempted several times but failed. When RTCP mode is ON & when we index the table, then the tool also moves in relation to the workpiece and thus it will end up in the same position. I also tried switching off TRAORI command before indexing the table and even tried the Cycle800 to loop. But it never satisfactorily worked. If In-house solution or Postability can provide such customisation then it will be great.

Thanks a lot for the inputs!!

 

[Chris In-House Solutions]

In-House Solutions can provide a post for this DMU70 machine.  Please ask your reseller to reach out to us for a quote.  

[Shiva.aero]

Thank you Chris!

Can In-house solutions provide post which outputs NC code with subroutine for 5 axis as discussed?

[Chris In-House Solutions]

As Colin explained subroutines with 5-Axis aren't typically output from Mastercam.  If you can provide us with some sample code of what you are expecting to see it might be something the post team can investigate setting up.  

You can do a toolpath transform in Mastercam but that really just saves you time from re-programming a similar feature on your part.

[gcode]

The multiaxis utility page will rotate your toolpaths as long as they are symmetrical

We have an ancient ( 2005 vintage) Mastercam post for a Siemens 840D and it posts good code.

This is a page from an Okuma horizontal mill program for an impeller which is why the axis of rotation

is the Y axis in this screen shot

 

 

 

 

[Guest]

On 6/6/2021 at 4:53 AM, Shiva.aero said:

I am a user of Esprit 2019 CAM for 5 axis programming of Aerospace components. Recently my employer decided to shift to Mastercam 2022

Our lathe programmer uses Esprit for multi turret and B-axis head Mill/Turn machines.

When he dos a Mill program he sparks up Mastercam.

[tmao]

I used to use Esprit on MAZAK integrex i machines 2-3 years ago, before that I was all the time using Mastercam on 5 axis mills. After several months discovering I decided to quit the job and found another 5 axis Mastercam programmer job..

Looks to me Esprit toolpath is more automated but less controllable, also the CAD side is a piece of shxt.. I really hate everytime I have to draw a line then make the line a "feature" then start to use it..

Display is also another problem to me, my eyes got hurt..

Mastercam needs more lines picked up and more options need setup, but the details control is way better than Esprit..

I really like Esprit's group toolpath feature that you can make a simple toolpath for all similar features as group and auto-trim them, that saves lots of time on simple contour programming.

My favorite function in Esprit is knit surface which provided by the CAD supplier (I forgot the name, same as my waterjet software).. In Mastercam power surface will do similar jobs..

 

[bd41612]

Shiva, you made "the right choice", based on my experience with Esprit.  Post support was terrible, and overall, the software did not live up to the expectations that they tried to sell us on.  What do you expect when the salesman says "we have the FANUC kernel embedded in our software, so you will get perfect code every time"?  Sounded great for 2 seconds, but how does the software know the difference between machine tools?  How does it know how the parameters are configured?  Their big selling point that they push is the saved process files.  But that can also be done with Mastercam using operational defaults and exported ops.  I had to suffer through it.  I rectified the situation by getting a new job, using Mastercam.

[Metallic]

I'd like to kinda revive this...a shop I am in talks with is trying to decide on CAM. They have a millturn coming and want to use esprit....I just can't understand it. Using both Hypermill and Esprit on their floor. What do you guys think of this? Is this as crazy as I think it is? Not only would I have to learn Hypermill, I would have to learn esprit. The guy thinks Mastercam 5-axis is 'entry level' and I about laughed in his face. Either way regardless of what they choose it seems having multiple CAM systems would be utterly awful to get up to speed with.

 

Just how good (or not) is Mastercam at Millturn on say an Integrex or a DMG NTX? As I have the Mastercam experience I would like to steer them in that direction...

[DUM1]

On 6/22/2021 at 6:32 AM, bd41612 said:

Post support was terrible, and overall, the software did not live up to the expectations

I'll second this statement x1000 , having been there before , tried 2 years to get a post right before scrapping it and going back to ONE CNC  .

the other guy supposed to use esprit on the integrex had to have a tech come in every time he tried to program it .

[#Rekd™]

1 hour ago, Metallic said:

 

Just how good (or not) is Mastercam at Millturn on say an Integrex or a DMG NTX? As I have the Mastercam experience I would like to steer them in that direction...

I have no experience but you might want to ask Bob W.

 

 

[cncappsjames]

...

we have the FANUC kernel embedded in our software, so you will get perfect code every time"

"FANUC kernel" 

First off,  I will never profess to know everything. That being said, I've got a solid 30 years of experience with FANUC controls ranging from the 3m/11m up through today's 30i Series and everything except the 3 digit Series (i.e. 310i, 320i, etc...) in between, and I've worked for a Machine Tool Builder or Machine Tool Dealer for 18 of those years... enough of the bonafides... in all that time, I have never even once heard "FANUC kernel". 

Now I'm intrigued. Am I missing something?

[bd41612]

20 hours ago, DUM1 said:

I'll second this statement x1000 , having been there before , tried 2 years to get a post right before scrapping it and going back to ONE CNC  .

the other guy supposed to use esprit on the integrex had to have a tech come in every time he tried to program it .

We had a post that Esprit was never able to fix (purchased post) they wanted to close the ticket after 6 months or so and re-open under a new ticket #.  Maybe it didn't look good to have an open incident for that amount of time.

15 hours ago, cncappsjames said:

 

 

"FANUC kernel" 

First off,  I will never profess to know everything. That being said, I've got a solid 30 years of experience with FANUC controls ranging from the 3m/11m up through today's 30i Series and everything except the 3 digit Series (i.e. 310i, 320i, etc...) in between, and I've worked for a Machine Tool Builder or Machine Tool Dealer for 18 of those years... enough of the bonafides... in all that time, I have never even once heard "FANUC kernel". 

Now I'm intrigued. Am I missing something?

It was a sales pitch.  Like I said, it sounded great for about 2 seconds, and then the bs detector went off.  My boss at the time, I think he fell for it.

[JeffreyS]

1 hour ago, bd41612 said:

We had a post that Esprit was never able to fix (purchased post) they wanted to close the ticket after 6 months or so and re-open under a new ticket #.  Maybe it didn't look good to have an open incident for that amount of time.

It all boils down to who touched the post as Colin would attest. I inherited a Postability post that was not aligned with a Siemens 840D that was supposedly a fully baked post. I found a company, worked with the post writer with my expected output, we got it all dialed in on the second iteration.

[gcode]

about 8 years ago I approached Esprit, NX, SolidCam and Hypermill  with a challenge

I wanted to see how well they could rough a family of impellers we build.

We had just purchased a new Okuma 5X HMC and needed a better way to program these impellers

They are made of mild steel and range in size from Ø30" to Ø60"  and 3 to 10 inches thick,

At the time I was roughing them with 5X curve toolpaths in Mastercam. It was a lot of work to program and I was not happy

with the results or the time it took me to do it.

 

I did give CNC a sample file and asked if MW's could handle this but never got anything back.

 

Espirt spent a lot of time on it, gave me a trial seat and posts for our Okuma HMC and VTM

They did mention an "Okuma kernel" in their sales pitch. I believe this is something in their posts and not something they get from Okuma (or Fanuc)

I didn't like anything about Espirt, especially it's extremely primitive CAD. You'll notice that every Espirt demo starts with "Import the model"

The toolpaths their AE came up with were unsatisfactory, and the quoted prices were breathtaking.

 

NX declined my challenge. At the time Tata Technologies handled the small business accounts (under $100 million annual revenue)

and the Tata AE's were not able or interested in doing the work.

 

SolidCam got on the phone and launched into a canned sales pitch about iMachining.

I felt like I was at Shady Sam's Used Cars on Hill Street in Oceanside.

I ended the call and that was that

It's too bad as I know a guy who does very solid work with SolidCam.

 

Hypermill came back in 3 days with an amazing file, and a bullet proof post and got the sale,

I really don't like hyperMill and roughing impellers is all I use it for.

It does an excellent job for what I use it for.

 

I haven't had time to take a serious shot at it, but I believe today's Mastercam/MW could do a very good job of roughing these

parts. 

 

 

 

[bd41612]

5 minutes ago, gcode said:

about 8 years ago I approached Esprit, NX, SolidCam and Hypermill  with a challenge

I wanted to see how well they could rough a family of impellers we build.

We had just purchased a new Okuma 5X HMC and needed a better way to program these impellers

They are made of mild steel and range in size for Ø30" to Ø60"  and 3 to 10 inches thick,

At the time I was roughing them with 5X curve toolpaths in Mastercam. It was a lot of work to program and I was not happy

with the results or the time it took me to do it.

 

I did give CNC a sample file and asked if MW's could handle this but never got anything back.

 

Espirt spent a lot of time on it, gave me a trial seat and posts for our Okuma HMC and VTM

They did mention an "Okuma kernel" in their sales pitch. I believe this is something in their posts and not something they get from Okuma (or Fanuc)

I didn't like anything about Espirt, especially it's extremely primitive CAD. You'll notice that every Espirt demo starts with "Import the model"

The toolpaths their AE came up with were unsatisfactory, and the quoted prices were breathtaking.

 

NX declined my challenge. At the time Tata Technologies handled the small business accounts (under $100 million annual revenue)

and the Tata AE's were not able or interested in doing the work.

 

SolidCam got on the phone and launched into a canned sales pitch about iMachining.

I felt like I was at Shady Sam's Used Cars on Hill Street in Oceanside.

I ended the call and that was that

It's too bad as I know a guy who does very solid work with SolidCam.

 

Hypermill came back in 3 days with an amazing file, a bullet proof post and got the sale,

I really don't like hyperMill and roughing impellers is all I use it for.

It does an excellent job for what I use it for.

 

I haven't had time to take a serious shot at it, but I believe today's Mastercam/MW could do a very good job of roughing these

parts. 

 

 

 

3 + 2 Automatic would probably be worth a shot.

[gcode]

52 minutes ago, bd41612 said:

3+ 2 Automatic would probably be worth a shot.

hypermIll generates a full 5X toolpath that reduced cycle times to 8 hours versus 30  or 40 with my old school MC files

I've done some experimenting with morph between curves and the pocketing toolpath (in MC2022)

Both showed promise.

The difference in power and capability between Master era 2013 and today is amazing

 

[#Rekd™]

24 minutes ago, gcode said:

SolidCam got on the phone and launched into a canned sales pitch about iMachining.

I felt like I was at Shady Sam's Used Cars on Hill Street in Oceanside.

I ended the call and that was that

It's too bad as I know a guy who does very solid work with SolidCam.

I had a sales call from SolidCam about 4 or 5 years ago and it was excellent. They had a screen sharing session and they were showing the software. During the session I emailed them a solid model that would require axis substitution in MC and they were able to program it with ease during the call. I still stayed with MC given the support for the software that is available.

[gcode]

2 hours ago, #Rekd™ said:

I had a sales call from SolidCam about 4 or 5 years ago and it was excellent. They had a screen sharing session and they were showing the software. During the session I emailed them a solid model that would require axis substitution in MC and they were able to program it with ease during the call. I still stayed with MC given the support for the software that is available.

The SolidCam sales guy really pissed me off

I told them ahead of time what I was looking for and what I wanted to see.

He launched straight into his canned sales pitch and despite my best efforts he could not be diverted from that.

[Metallic]

31 minutes ago, gcode said:

The SolidCam sales guy really pissed me off

I told them ahead of time what I was looking for and what I wanted to see.

He launched straight into his canned sales pitch and despite my best efforts he could not be diverted from that.

Wouldn't this family of parts be an ideal application for the BladeExpert add-in for Mastercam? I know it aint cheap but it also ain't cheap to sit around for 8 hours programming a roughing blade op when the add-in could do it in 20 minutes.

 

That is my beef with the company I was referring to getting HyperMill. They bought Hypermill strictly for 3+2 work....which I am like "okay cool but that is better for 5x simultaneous". Saying Mastercam is a slouch in 5x is disingenuous and that is the narrative they are pushing. Especially considering they aren't doing much simultaneous, almost any CAM package out there could handle 3+2 roughing and finishing

 

I did have a Hypermill rep in my shop a few months ago and was very interested in it for some of our 5x stuff...the quote was astronomical to say the least. But I am still considering it for future if I stay in my current role.

[gcode]

40 minutes ago, Metallic said:

Saying Mastercam is a slouch in 5x is disingenuous and that is the narrative they are pushing. Especially considering they aren't doing much simultaneous, almost any CAM package out there could handle 3+2 roughing and finishing

HyperMill is very good at 3+2. It's not easy to use, but very powerful.

I know this is heresy and goes against conventional wisdom, but I found hyperMill's swarf toolpaths to be primitive at best.

We dropped maintenance in 2017 so my knowledge is dated, but back then Mastercam/ModuleWorks ran rings hyperMill

where swarf was concerned

[cncappsjames]

3 hours ago, gcode said:

about 8 years ago I approached Esprit, NX, SolidCam and Hypermill  with a challenge

I wanted to see how well they could rough a family of impellers we build.

Esprit... not a fan. CAD is unacceptable. They are too much "you must do it this way" for my liking. Reminds me of GibbSCAM. Multitasking Lathes and EDM are a different story and is good in those arenas IMHO.

NX... too much like CATIA. Very cumbersome. Lots of menus. Awesome Engineering software though. Pass.

SolidCAM. Pure, unadulterated bovine excrement. We've got a few customers with it. Nothing but problems on the CAM output side. Even their drilling cycles lack adequate controls. HARD pass.

Hypermill. I have nothing good to say. Go with Tebis or PowerMill if you're going to spend that kind of dough on CAM.